User’s Guide

Version 6.0 May 2016


© Copyright 2004-2016
ALL RIGHTS RESERVED

Table of Contents

TABLE OF CONTENTS ........................................................................................III

1. WELCOME ..................................................................................................... 1

WELCOME TO ENROUTE ................................................................................... 1

WHATS NEW IN ENROUTE ................................................................................ 1

RECOMMENDED SYSTEM REQUIREMENTS .......................................................... 4

HARDWARE KEY ............................................................................................... 5

INSTALLING THE SOFTWARE .............................................................................. 5

ENROUTE 5 SUPPORT SERVICES ...................................................................... 6

2. GETTING STARTED ...................................................................................... 9

WORKFLOW...................................................................................................... 9

BASIC ELEMENTS OF ENROUTE......................................................................... 9

WORKING WITH VIEWS .................................................................................... 10

MENUS........................................................................................................... 10

TOOLBARS ..................................................................................................... 10

CHANGING UNITS ........................................................................................... 11

STATUS LINE .................................................................................................. 11

USING SCROLL BARS ...................................................................................... 12

PRECISION INPUT CENTER .............................................................................. 12

USING SNAPS ................................................................................................. 13

GUIDELINES ................................................................................................... 14

EDIT GUIDELINES DIALOG ............................................................................... 14

CHANGING THE VIEW ...................................................................................... 16

ZOOM COMMANDS .......................................................................................... 17

REDRAW ........................................................................................................ 17

VIEW SETUP ................................................................................................... 18

UNDO AND REDO ............................................................................................ 18

WORKING WITH LAYERS .................................................................................. 18

CHANGE LAYER .............................................................................................. 20

USING HELP ................................................................................................... 21

PREFERENCES ............................................................................................... 21

EXITING THE SOFTWARE ................................................................................. 30

3. TOOLBARS AND COMMAND ICONS ........................................................ 31

OTHER COMMAND ICONS ................................................................................ 51

4. WORKING WITH DRAWINGS ..................................................................... 57

CREATING NEW DRAWINGS............................................................................. 57

USING PLATE TEMPLATES ............................................................................... 62

OPENING A DRAWING...................................................................................... 62

SAVING A DRAWING ........................................................................................ 63

CLOSING A DRAWING ...................................................................................... 63

IMPORTING A DESIGN ..................................................................................... 63

EXPORTING DESIGN INFORMATION .................................................................. 64

PRINTING ....................................................................................................... 64

CALCULATOR ................................................................................................. 65

SNAPSHOT ..................................................................................................... 65

MEASURE ...................................................................................................... 65

5. CREATING CONTOURS ............................................................................. 67

LINE, POLYARC BEZIER CURVE OR DRAW A CURVED CONTOUR ....................... 67

RECTANGLE ................................................................................................... 72

CIRCLE .......................................................................................................... 74

ARC............................................................................................................... 75

ELLIPSE ......................................................................................................... 76

COMPONENT CREATOR .................................................................................. 78

POLYGON ...................................................................................................... 81

TEXT ............................................................................................................. 82

GEOMETRY CREATION WIZARD ....................................................................... 86

CONE WIZARD ............................................................................................... 86

BOXSTER ....................................................................................................... 88

DIMENSIONS .................................................................................................. 92

6. CONTOUR EDITING .................................................................................... 95

EDITING POINTS ON A CONTOUR ..................................................................... 95

EXTENDING CONTOURS ................................................................................ 100

TRIMMING CONTOURS .................................................................................. 102

FILLETING CONTOURS .................................................................................. 104

JOINING CONTOURS ..................................................................................... 107

OFFSET CONTOURS ..................................................................................... 107

PARTIAL OFFSET CONTOURS ........................................................................ 108

MERGING SELECTED OPEN CONTOURS......................................................... 109

EXPLODE SELECTED CONTOURS................................................................... 109

CONVERTING CURVES TO ARCS .................................................................... 110

REVERSE OPEN CONTOURS ......................................................................... 110

CREATING MULTIPLE COPIES OF A CONTOUR ................................................ 111

VECTORIZING BITMAPS ................................................................................. 116

CLEANING UCONTOURS............................................................................. 117

7. ARRANGING CONTOURS ........................................................................ 119

SELECTING CONTOURS ................................................................................ 119

CUTTING, COPYING AND PASTING CONTOURS ............................................... 119

DELETING CONTOURS .................................................................................. 120

GROUPING AND UNGROUPING CONTOURS ..................................................... 121

MOVING, SCALINGAND ROTATING OBJECTS ................................................. 121

MOVE TOOL ................................................................................................. 125

SCALE TOOL ................................................................................................ 126

ROTATE TOOL .............................................................................................. 130

DISTORT CONTOURS .................................................................................... 133

ALIGNING OBJECTS ...................................................................................... 138

WELDING CONTOURS ................................................................................... 139

USING THE CUT BY LINE TOOL....................................................................... 142

NEST TOOL .................................................................................................. 143

NEST SUMMARY REPORT .............................................................................. 149

8. WORKING WITH TOOLPATHS................................................................. 153

OVERVIEW ................................................................................................... 153

CREATING ROUTING OFFSET TOOLPATHS ...................................................... 154

CREATING OPEN CONTOUR OFFSET TOOLPATHS ........................................... 164

KERF COMPENSATION TOOLPATHS................................................................ 167

DAISY CHAIN TOOLPATHS ............................................................................. 168

HATCH FILL .................................................................................................. 169

CREATING ISLAND FILL TOOLPATHS ............................................................... 173

SPIRAL FILL TOOLPATHS ............................................................................... 176

DRILL TOOLS ................................................................................................ 178

CREATING SLOT TOOLPATHS ........................................................................ 187

CREATING AN ENGRAVE TOOLPATH ............................................................... 188

SQUARE CORNER FOR EXTERNAL 3D ENGRAVE............................................. 189

CREATING PYRAMID TOOLPATHS ................................................................... 191

EDITING TOOLPATHS..................................................................................... 193

EDITING THE TOOLPATH PLAN ....................................................................... 194

EDITING ENTRY/EXIT POINTS ........................................................................ 195

EDITING BRIDGES ......................................................................................... 197

DISTORTING TOOLPATHS .............................................................................. 199

DELETE TOOLPATHS ..................................................................................... 202

PROJECT TOOLPATHS ................................................................................... 202

9. PREVIEWING OUTPUT ............................................................................. 205

SIMULATING OUTPUT IN 2D ........................................................................... 205

SIMULATING OUTPUT USING AN ORTHOGRAPHIC VIEW ................................... 207

CREATE RENDERED VIEW OF TOOLPATHS ..................................................... 208

10. CONFIGURING THE SOFTWARE ............................................................ 211

CONFIGURING MACHINE DRIVERS ................................................................. 211

EDITING THE MATERIAL LIBRARY ................................................................... 217

EDITING THE TOOL LIBRARY .......................................................................... 218

11. OUTPUT TO MACHINE ............................................................................. 223

SETTING THE TOOLPATH ORDER ................................................................... 223

GENERATING OUTPUT................................................................................... 224

12. 3D SURFACES AND 3D TOOLPATHS ..................................................... 231

INTRODUCTION ............................................................................................. 231

3D SURFACE APPLICATIONS ......................................................................... 231

CREATING 3D SURFACES.............................................................................. 232

CREATING OUTPUT FOR 3D SURFACES ......................................................... 232

13. CREATING RELIEFS ................................................................................. 233

CREATING A RELIEF...................................................................................... 233

RELIEF SHAPE ............................................................................................. 233

RELIEF OPTIONS .......................................................................................... 234

APPLICATION METHOD.................................................................................. 236

RELIEF PARAMETERS ................................................................................... 239

USING THE RELIEF DIALOG ........................................................................... 242

14. REVOLUTIONS AND EXTRUSIONS ........................................................ 247

INTRODUCTION ............................................................................................. 247

REVOLVE ..................................................................................................... 247

SPIN ............................................................................................................ 253

EXTRUDE ..................................................................................................... 263

SWEEP TWO RAILS....................................................................................... 272

15. CHAMFERING ........................................................................................... 281

INTRODUCTION ............................................................................................. 281

STANDARD CHAMFER ................................................................................... 281

CHAMFER CENTERLINE................................................................................. 288

BAROQUE CHAMFER..................................................................................... 292

16. USING 3D MESHES .................................................................................. 295

INTRODUCTION ............................................................................................. 295

USING 3D MESHES FROM OTHER APPLICATIONS ........................................... 296

CREATING 3D MESHES WITH ENROUTE TOOLS ............................................. 296

SLICING MESHES.......................................................................................... 298

APPLYING MESHES TO A RELIEF.................................................................... 304

UNWRAPPING MESHES FOR ROTARY AXIS SUPPORT...................................... 309

17. MODIFYING AND COMBINING RELIEFS ................................................ 315

INTRODUCTION ............................................................................................. 315

SELECTING RELIEFS ..................................................................................... 315

CUTTING, COPYING AND PASTING RELIEFS .................................................... 315

DELETING RELIEF OBJECTS .......................................................................... 316

CLEARING RELIEFS....................................................................................... 316

MOVING RELIEFS ......................................................................................... 317

ROTATING RELIEFS ...................................................................................... 318

SCALING RELIEFS......................................................................................... 319

FIT RELIEF TO PLATE.................................................................................... 320

SMOOTHING RELIEFS ................................................................................... 320

INVERTING RELIEFS ...................................................................................... 321

CREATE A MESH SURFACE FROM A RELIEF ..................................................... 324

OFFSET RELIEF SURFACE............................................................................. 326

MERGE RELIEFS........................................................................................... 327

COMBINE RELIEFS ........................................................................................ 329

EXTRACT RELIEF SLICES .............................................................................. 329

18. USING BITMAPS ....................................................................................... 333

INTRODUCTION ............................................................................................. 333

APPLYING BITMAPS TO A RELIEF.................................................................... 333

USING A MASK.............................................................................................. 335

3D EFFECTS USING BITMAPS ........................................................................ 336

19. TEXTURE TOOLS...................................................................................... 339

INTRODUCTION ............................................................................................. 339

PARAMETRIC TEXTURES ............................................................................... 341

SYMMETRIC PARAMETRIC TEXTURES ............................................................. 351

RAPID TEXTURE ........................................................................................... 352

RAPID TEXTURE DIALOG ............................................................................... 355

STEP BY STEP EXAMPLES ............................................................................. 358

CREATING AND CUTTING CONTINUOUS PANELS ............................................. 371

RAPID PICTURE TOOL ................................................................................... 380

20. RELIEF EDIT TOOLS................................................................................. 389

EDIT RELIEF TOOLBAR .................................................................................. 389

FADE AND SHRINK ........................................................................................ 390

BUILD PARAMETER ....................................................................................... 391

21. 3D TOOLPATHS ........................................................................................ 393

INTRODUCTION ............................................................................................. 393

3D TOOLPATH STRATEGIES .......................................................................... 393

3D TOOLPATH STRATEGY PARAMETER .......................................................... 394

3D TOOLPATHS WITH A STEP ROUGH ............................................................ 403

ENGRAVE TOOLPATHS ON A RELIEF ............................................................... 410

3D SIMULATION OF TOOLPATHS .................................................................... 413

22. AUTOMATIC TOOLPATHS ....................................................................... 417

INTRODUCTION ............................................................................................. 417

OVERVIEW OF THE ATP PROCESS................................................................. 418

ACTIVATING THE ATP DIALOG ....................................................................... 419

THE ATP DIALOG ......................................................................................... 420

SELECTING THE ACTIVE DESIGN APPLICATION ............................................... 421

SELECTING FILES TO PROCESS ..................................................................... 422

LAYER MAPPING ........................................................................................... 424

ORDERING AND NESTING .............................................................................. 430

ATP SETUP.................................................................................................. 436

EXAMPLE STEPS TO PROCESS YOUR FILES ................................................... 439

LABELS IN ENROUTE..................................................................................... 442

23. KEYBOARD SHORTCUTS ........................................................................ 457

24. INDEX ......................................................................................................... 459

Software License Agreement

Carefully read the following terms and conditions sign and return as accepting these terms and conditions.

This is a legal agreement between you, the end user (either an individual or an entity), and SA International, Inc. If you do not agree with the following, you should promptly return the package. Use of this program indicates your acceptance of the terms and conditions stated below.

The enclosed computer program "Software" is licensed, not sold, to you by SA International, Inc., for use on a non- exclusive, non-transferable basis, only under the following terms, and SA International, Inc., reserves any rights not expressly granted to you. You may not disclose to any third party any confidential information concerning the Software or SA International, Inc. or use such confidential information to the detriment of SA International, Inc...

1. License.

This software is protected by the United States Copyright Law and International Treaty Provisions. Therefore, you must treat the Software just as you would any other copyrighted material, such as a book. This license allows you to:

(a) Make one copy of the Software in machine readable form; provided that such a copy of the original may be used solely for backup purposes. As an express condition of this License, you must reproduce on each copy of the SA International, Inc., copyright notice and any other proprietary legends on the original copy supplied by SA International, Inc.

(b) Transfer the Software and all rights under this License to another party together with a copy of this License and all written materials accompanying the Software provided you give SA International, Inc., written notice of the transfer and the other party reads and agrees to accept the terms and conditions of this License.

(c) Use this Software on a single computer only, but may transfer it to another computer as long as it is used on only one computer at a time. “In Use” constitutes being loaded onto either temporary (i.e., RAM) or permanent memory (e.g., hard disk, CD-ROM or other storage device) of a computer.

2. Restrictions.

You may NOT distribute copies of the Software to others or electronically transfer the Software from one computer to another over a network. You may not de-compile, reverse engineer, disassemble or otherwise reduce the Software to a human perceivable form. You may not modify, adapt, transfer, rent, lease, loan, resell for profit, distribute, network or create derivative works based upon the software or any part thereof.

3. Termination.

This License is effective until terminated. This License will terminate immediately if you fail to comply with any of its provisions. Upon termination, you must return the Software, and all copies thereof, to SA International, Inc., and you may terminate this License at any time by doing so.

4. Export Law Assurances.

You agree that neither the Software nor any direct product thereof will be transferred or exported, directly or indirectly, into any country prohibited by the United States Export Administration Act or any international export laws and the restrictions and regulations thereunder, nor will it be used for any purposes prohibited by the Act or laws.

5. Warranty Disclaimer, Limitation of Remedies and Damages.

In no event will SA International, Inc., be liable for any damages, including infringement, lost data, lost profits, cost of cover or other special, incidental, consequential or indirect damages arising from the use of the program however caused and on any theory of liability. This limitation will apply even if SA International, Inc., or an authorized dealer or distributor has been advised of the possibility of such damage. SA International, Inc. MAKES NO WARRANTY,

Welcome

EXPRESS OR IMPLIED, WITH RESPECT TO THE SOFTWARE, AND DISCLAIMS, WITHOUT LIMITATION, ANY IMPLIED WARRANTY OF MERCHANTIBILITY OR FITNESS FOR A PARTICULAR PURPOSE. SA International, Inc. does not warrant any drivers for plotting, scanning or either devices. These drivers are provided for our customers as a service only, and were developed using information provided to us at the time by the equipment manufacturers.

SA International, Inc. is not responsible for any typographical errors in the software or in the documentation.

6. General.

If you are a U.S. Government end-user, this License of the Software conveys only "RESTRICTED RIGHTS," and its use, disclosure, and duplication are subject to Federal Acquisition Regulations, 52.227-7013(c) (1) (ii). This License will be construed under the laws of the State of Pennsylvania, except for that body of law dealing with conflicts of law, if obtained in the U.S., or the laws of jurisdiction where obtained, if obtained outside the U.S. If any provision of this License is held by a court of competent jurisdiction to be contrary to law, that provision of this License will remain in full force and effect.

© Copyright 2016 by SA International, Inc. and Artistic Automation, Inc. All rights reserved. No part of this publication may be reproduced, stored in a retrieval system or transmitted, in any form or by any means, electronic, mechanical, photocopy, recording or otherwise, without the prior written permission of the publisher. Printed in the United States of America. The information in this manual is subject to change without notice and does not represent a commitment on the part of SA International, Inc.

Acrobat® Reader Copyright© 1987-2016 Adobe Systems Incorporated. All rights reserved. Adobe and Acrobat are trademarks of Adobe Systems Incorporated which may be registered in certain jurisdictions. PostScript® software Copyright© 1984-1998 Adobe Systems Incorporated. All rights reserved.

Flexi, FlexiFAMILY, FlexiSIGN-Pro, FlexiSIGN Plus, FlexiEXPERT, FlexiSIGN, FlexiLETTER, FlexiDESIGNER, FlexiCUT, FlexiENGRAVE, PhotoPRINT Server, PhotoPRINT, PhotoPRINT SE, EnRoute-Pro, EnRoute Plus, EnRoute and/or other SA International products referenced herein are either trademarks or registered trademarks of SA International, Inc. Illustrator is a registered trademark of Adobe Systems Incorporated. FreeHand is a registered trademark of Macromedia Corporation. CorelDRAW! is a trademark of Corel Systems Corporation. AppleTalk, ImageWriter, LaserWriter, and Macintosh are registered trademarks of Apple Computer, Inc. Windows is a registered trademark of Microsoft Corporation. The names of actual companies and products mentioned herein may be the trademarks and/or registered trademarks of their respective owners. Adobe® is a trademark of Adobe Systems Incorporated or its subsidiaries and may be registered in certain jurisdictions. PostScript® is a trademark of Adobe Systems Incorporated or its subsidiaries and may be registered in certain jurisdictions.

SA International, Inc.

1. Welcome

Welcome to EnRoute

EnRoute is a CAD/CAM application that will allow you to create a wide range of finished products. With it you can create two-dimensional (2D) and three dimensional (3D) designs and then create all of the toolpaths necessary to produce the parts using your CNC machine.
EnRoute includes many productivity-enhancing features that simplify the design process. Templates can be saved at many points in the process so that your decisions regarding specific design features, material types, tool choices, toolpath strategies, and output ordering may be saved for future use.
The goal of your design process is to produce finished parts efficiently and economically. EnRoute’s wide range of toolpath creation tools, nesting, and output ordering options help you accomplish this goal.
This manual is intended to serve as a starting point for learning EnRoute. It is also available in the form of online HTML Help in the software. Many other training options are available from SAI for those who would like additional assistance in taking advantage of EnRoute’s capabilities.
In this chapter, you will learn about:

 What’s new in EnRoute

 Recommended System Requirements

 Hardware Key

 Installing the Software

 EnRoute 6 Support Services

What’s new in EnRoute

Version 6 of EnRoute includes many significant changes and improvements from previous versions.

INTERFACE AND GENERAL IMPROVEMENTS

Keyless Security – EnRoute no longer requires a dongle! Now use InstallManagerCloud.exe to change between versions.

Improved redrawing of contours and toolpaths-This speeds up the drawing and redrawing of contours, toolpaths, and meshes. Every time you zoom, pan, switch views, or redraw the drawing, it will be faster. For people who create lots of toolpaths (3D) it would probably be worth the price of admission all by itself.

Simulation improvements – The new simulation engine gives the ability to use wood textures and

Welcome Page 1

other types of materials to provide a more realistic view of the finished piece. We have also improved EnRoute’s simulation of cutting so that users can better visualize how the piece will cut. EnRoute now does a better job of utilizing the capabilities of the computer’s video card to create the simulation.

Rendering enhancements- Relief rendering in EnRoute has been improved also. The perspective view of reliefs does a better job of showing the relief from all angles so that users can visualize their design as they are working on it.

Dynamic Language Switching – Access to languages other than English in EnRoute used to require the user to change the locale on her computer. Now you simply select the language from a menu item and the language of choice is activated.

On-demand movies - When you are getting started with EnRoute, you need to be able to get your questions about a specific tool answered right now. EnRoute 6 puts the answers at your fingertips. Right click on a button and a short movie explaining that tool will play. These days, watching a movie to learn about software functionality is the choice of most users and we make it as easy as pointing and clicking.

Support for the Lathe in the interface – The plate setup dialog now includes easy support for defining the plate to accommodate a rotary axis design of a specific diameter. It is then easy to switch between “wrapped” and “unwrapped” mode when you are creating the design.

NEW DESIGN TOOLS

Model Stacker – This new tool gives you the ability to slice a mesh in any direction and then automatically create 2D slices that can quickly be nested and cut out. The cut slices can be stacked to create a unique version of your model. EnRoute takes care of numbering the slices so you can keep them in order, and it is also easy to create holes in each slice to fit one or more alignment rods for assembling your masterpiece.

New Tangential Snap – Allow you to create tangent lines between two circles.

New Intersection Snap - New snap to help identify overlapping line segments. To aid with cleanup of imported contours with extra lines.

Improved Support for Single-Stroke Fonts – In addition to our built-in fonts, we have added support for a more industry standard technique that allows users to utilize single-stroke fonts from other sources such as One Line Fonts. These fonts are handy for marking applications and are efficient to cut.

Zoom to Selection now works for all active views at once. A simple change but surprisingly handy.

Point Edit for Arcs Stays Arcs – If point editing changes are made to objects made of lines and arcs, the line segments remain line and arc after editing. Helps with editing shapes for letter bending and reducing arcs in output files.

New Concentric or Eccentric Cone Wizard tool – Allows for cones to be created that have the same center point or offset center points.

Text Tool Improvements – We went through our text tool and made several improvements that make it much easier to work with larger text blocks. When typing and editing text, we got rid of extra text redraws. In addition, it is now easy to copy and paste text strings from other sources using the Windows clipboard. Again, a simple improvement that makes all the difference.

Page 2 Welcome

TOOLPATHING and OUTPUT

Support for paneling with output for large jobs – This new tool makes it simple to accommodate designs that are too big for your table, or too big for the material you want to use. Just define your panel sizes and EnRoute takes care of breaking up the output.

Contour Editing – when a user deletes a point to simplify a contour, if the point is between two arcs, the remaining segments will include just one arc in place of the two arcs.

Component Creator Wizard – This is a tool that allow you to create interlocking components that can be used to create shelves and other objects.

Output Orientation Rotation added to ATP – for flipping the output axis during ATP output. Can show as Long X on screen but output as Long Y.

Right Click – The Create Toolpath menu now includes Open Contour Offset.

ENROUTE 3D SURFACE CREATION FEATURES (EnRoute Pro)

Relief Slicing – The Relief Slicing tool has been completely reworked to make it easier to use, and more reliable to create slices. Whether you are creating one slice or a hundred, this tool makes it simple.

Relief Slice Masking – One of the best features of the new slicing tool is the ability to automatically create masking contours for each slice that can be used to apply toolpaths only where they are necessary for milling the 3D surface of the relief. Creating these masks used to be a pretty laborious manual task to be done after the slices were created.

Vertical Slicing of Reliefs – The Component Maker also now makes it easy to slice up a relief vertically as well as horizontally. This can be used as a way to build large models more quickly, or as a way to get a new effect from your design.

Unwrap a 3D Model for Rotary Cutting - Adds the ability to unwrap a 3D model onto a relief so that it can be wrapped back to a lathe for output. This allows 3D models to be cut out on a rotary axis tool without distortion. If you have a rotary axis machine, you can now mill out full models without the need to split them into a top half and a bottom half.

TEXTURES

Symmetric parametric textures – A new set of parametric textures is available that are automatically symmetric for any size. You can create amazing surface textures and then be able to either make several identical panels or reproduce the panels some other way – and they always match up seamlessly right to left and top to bottom.

Simplified Rapid Texture- Improvements that make it easier to get good results without having to totally understand what you are doing. No Seed Contour Required.

Symmetric Rapid Texture- It is now easier to create Symmetric Rapid Texture Features that works with any panel size and is easy to use and hard to screw up.

Rapid Texture Templates- Templates have been updated to include 19 starting textures.

New Parametric Texture Templates – We have added many new parametric textures that work in both inches and MM to help get you started. A new Bamboo Parametric Texture has been added.

Welcome Page 3

Bug Fixes/Misc. –

 Fixes ATP Nesting issue for Block Nesting with ATP.

 Updated support for iCut XML files.

 Updated support for Caldera.

 Update for DWG/DXF for certain objects.

Changes to Product Levels – Products levels get some new functionality with EnRoute 6

Entry- Now includes Explode, Layer Editing and Dynamic Nesting. 3D Engrave is an Option.

Basic- Includes 3D Simulation and Dynamic Nesting.

Plus- Now includes Rapid Texture and ATP Lite for Nesting and Output at the same time.

Pro – Now includes full ATP and Labeling.

Fab – There is now only one Fab Product and True Shape Nesting is an Option.

Recommended System Requirements

Before you begin installing the software, read the hardware requirements below. For optimal performance we suggest that your system meet the recommended requirements. As with all computer software, systems with faster processors, more RAM, and greater amounts of storage space allow you to work with larger files and keep your processing time to a minimum.

 

Windows

Processor

Intel Core i5 or comparable.

RAM

1 GB minimum, 4BG recommended

Install Space

300 MB

Working Disk Space

4 GB

Operating System

Windows 7/8/10

Video

1024 x 768 resolution with 24-bit color. We also recommend a dedicated video card with on-board RAM.

Page 4 Welcome

Hardware Key

Previous versions of EnRoute required the use of a hardware key for licensing purposes. EnRoute 6 utilizes a licensing system that is tied to your computer, and so it does not require the use of a hardware key. For the great majority of our users, this is a very welcome change and removes the added complication of having to keep track of their key.
The one drawback of not using a hardware key is that it reduces the portability of an EnRoute license. Since the license was tied to the key, it was easy for a user to move from computer to computer just by moving the key to a different computer. With the keyless system it is still possible to move the license between computers, but it requires the user to log in to their account on the SAI licensing website to disable one computer and then enable a different computer.
It is still possible to use a hardware key with your copy of EnRoute 6. In this case, the license will be tied to the key rather than any one computer. This will require that the USB key be attached to the computer in order for EnRoute to be usable on that computer. If you would like to utilize a hardware key to license your copy of EnRoute, please contact EnRoute support (http://www.enroutesoftware.com/enroute-professional-resources) in order to purchase a hardware key.

Installing the Software

You most likely downloaded the EnRoute installer as an executable file from the SAi website. To start the installation, simply double click on the installer.
The EnRoute installer will lead you through several steps to install the software in the desired location on your computer. You will also have the opportunity to install the appropriate password for your version of EnRoute during the installation process.

Following are the installer steps along with an explanation of the appropriate action.

1.

Welcome to the EnRoute

Setup Wizard

Click Next to continue.

2.

License Agreement

This provides the agreement between you and SA International, Inc. for the license of EnRoute. You are encouraged to read this agreement in full. If you agree, click the I Agree button to continue with the installation.

3.

Choose Install Location

The default location is c:\EnRoute6\. EnRoute is a self- contained application so all of the files required to run the software are included in the install folder. You can choose another location or another name for the EnRoute folder. After choosing the desired install folder click Next.

4.

Choose Start Menu

Folder

The default folder name is EnRoute6. You may choose to call it something else if you wish. After defining the start menu folder name, click Next.

5.

Installing

Installation of the software will start.

Welcome Page 5

6.

Do you prefer to work in millimeters?

You will be prompted with this question. If you do most of your work in millimeters, click Yes. Some of the initial default

values in EnRoute will be defined appropriately based on your choice.

7.

Activation Code

You will be prompted to enter an activation code that was provided either by SAi or by your dealer when you purchased the software. After entering the code, press the Next button and the installer will communicate with the SAi server to confirm the license for your computer. Press Next again to see the details of the license, and then press Finish to complete the licensing process.

8.

Installation Complete

After all of the files have been installed, you will be notified that the installation is complete. Click Next and then click on Finish in the dialog that will exit the installation wizard.

EnRoute 5 Support Services

On-Line Support Services

SA International recognizes the pressures you must endure with your business, computers and new software. There are times when you need help, which we understand. SA International is available to help you with your technical question, as well as your “How To” problems with our software. A variety of help methods are available to fit your budget, as well as your urgency to offer true value and peace of mind.

 One of the new features in EnRoute 6 is that every button provides easy access to an online video that explains the use of that feature. Just right click on the button, and if your computer has access to the Internet, the video will be activated.

EnRoute offers numerous free support options which include access to our YouTube channel, manuals and tech support e-mail. Check out our EnRoute Adventures Blog outlining projects step by step while inspiring new ideas for your future projects.
EnRoute also offers training options that fit a range of budgets and preferences. If you are a do-it- yourself learner take advantage of a training DVD or on-line one-on-one option with one of our application experts. If you prefer to be with colleagues and work among the energy of a group go for a workshop experience. See the website for information on the latest workshops.

Support in North America

New and upgraded products qualify for 90 Days Free Support from the date of purchase. During these first 90 days, unlimited free technical support is available in North America by calling our Technical Support Team Line: 800.229.9044

Page 6 Welcome

Technical Support Hours: Monday – Friday 8:00 AM – 5:00PM MST

The best way to contact SAi support is by going to www.EnRouteSoftware.com and then going to the Support page. This page provides a form for submitting an email question, and it also provides access to a wide range of free instructional videos that may well answer your questions. We also maintain an EnRoute forum that allows users to exchange information about EnRoute. The forum gives you a chance to help others with their questions, and to get answers to your questions.

EnRoute Workshops

One great way to learn EnRoute by working directly with EnRoute experts is to attend one of the many workshops we have in various locations in North America throughout the year. At the workshops you not only get the chance to work with our experts, you also get the chance to exchange tips and tricks with other EnRoute users. Check out the Support page on the web site for information about upcoming workshops.

US World Headquarters

5296 S. Commerce Dr. Suite 102
Murray, Utah 84107 USA Tel: 800.229.9066
Tel: 800.229.9068
Fax: 801.401.7234

European Office

Leuvensesteenweg 555 bus 3

This email address is being protected from spambots. You need JavaScript enabled to view it.This email address is being protected from spambots. You need JavaScript enabled to view it.
Tel: +32.2.725.5295
Fax: +32.2.725.2809

South / Central America

Rua Jose Osvaldo, 341
CEP 02250-010-
Sao Paulo-SP-Brazil
+ 32.2.725.5295

Welcome Page 7

Page 8 Welcome

2. Getting Started

Workflow



Design Toolpath Output

The graphic above illustrates the basic concept for completing a project in EnRoute. It may seem simplistic, but it does have a valuable practical use. When you are working in EnRoute, you are at all times within one of these steps of the process, and it is important to always understand where you are in the process. In the Design phase you are typically creating 2D contours for your design. You might also be creating a relief surface or a mesh object. Everything you do to define the geometry and surfaces of your design is part of the design process.
After completing the design, you are ready to create the toolpaths for cutting out the design. In this stage, it is important to understand such things as the material you plan to use, the tools you have available, and the quality of the finish required on the cut edges and surfaces of the parts. Output to the machine requires you to select the correct output driver, and to make sure that the configuration in EnRoute matches your specific machine.

Basic Elements of EnRoute

The main display area shows a view of the workspace. It can display a Top, Right, Front or Perspective view of the workspace, or all four views at the same time. Although you will likely do the majority of your work in the top view, it is often very convenient to be able to view contours and toolpaths from other views in order to see how they relate to each other.

Getting Started Page 9

Working with Views

To maximize a view, double-click on the name of the view that appears in its upper left corner. Double- clicking on the name a second time returns you to the four-view layout.
You can also toggle between the top view and the perspective view using the F12 key.

Menus

All tools and options are available by selecting them from the menus at the top of the screen. File

Edit, View, etc. Click on the Menu name to open the menu.

Toolbars

In addition to locating the tools through the menus you can also find the tools readily available on the toolbars. Some of the toolbars contain flyout Toolbars. The flyout Toolbar is a group of tools that share the same space on a toolbar, the entire group of tools “fly out” when you press and hold the first tool. A small yellow triangle in the lower right corner identifies the first tool in a fly-out toolbar.

Hiding and Displaying Toolbars

Menu: Setup / Toolbars

The user has the option to turn off some or all of the toolbars associated with this program. If there is a check mark in front of the toolbar’s name, the toolbar is turned ON.

Resetting Toolbars

Menu: Setup / Toolbars / Reset to Defaults

Select Reset to Defaults if you would like to set the toolbars back to their original position.

Using Toolbar Flyout Menus


Many toolbar icons have a small yellow triangle in their lower right corner indicating that a flyout menu for the tool exists.
A quick click on the toolbar icons will activate that particular tool. Click and hold for a short time in order to access the flyout menu containing several more tools.

Page 10 Getting Started

If you click on the edge of a flyout menu and drag it, the menu will “tear off” and form a floating menu.

This allows you to display the flyout function during that session, or until you close that toolbar.

Rulers

Menu: View / View Ruler

Rulers appear along the top and left side of a view to help you measure and align objects. Rulers can be activated for the top, right and front views from the View menu. The rulers can be very helpful in keeping track of where you are in a design as you move around in the design during the design process.
The rulers are also a handy way to bring guidelines into the work area, by just clicking on a ruler and dragging the guideline into the design.

Displaying and Hiding Rulers

Menu: View / View Ruler

To show or hide the rulers, from the View menu, point to View Ruler and click Top, Right or Front view.

Changing Units

Menu: Setup / Preferences / Units tab

To change the units used for all the drawing elements in your design, from the View menu, click on

Preferences and choose the Units Tab. Select the unit of measure desired.

Status Line

The status line along the bottom of the display provides a number of pieces of information. On the left side of the status bar the current coordinates of the cursor are constantly updated. If objects are selected, their size is displayed to the right of the coordinates.
During operations that require more than a moment or two of processing, a status bar is activated to provide feedback of the progress of the task.

Getting Started Page 11

Using Scroll Bars

Menu: View / View Scroll Bars


Scroll bars are horizontal and vertical bars located on the bottom and left side of your design area. Use them to scroll the design area.

Click the arrows on both sides to scroll the design area in small increments

Click the blank area to move the design area in large increments

Click and drag to scroll the design

To toggle scroll bars on and off, from the View Menu, select the View scroll bars option.

Precision Input Center

Menu: View

Toolbar: Settings

The Precision Input Center is utilized as an interface for some of EnRoute’s activities. It can be activated at any time by pressing F2 or clicking on the icon in the Settings toolbar. Activating the Precision Input Center by using F2 provides a simple method to move, scale or rotate selected objects. Other, more detailed, methods for moving, scaling, and rotating selected objects are also available, and are discussed in other sections of this manual.

For example, if you want to move the selection to a specific location, press F2 and select the Move
tab. Then enter the coordinates for the new location of the selection.

Page 12 Getting Started

Using Snaps

Menu: Setup / Snaps


Snaps allow you to select specific points during geometry construction and editing activities. Within most of the drawing commands, if you have snaps activated then as you move the
cursor around on the screen the cursor will snap to drawing element points that meet the criteria of the snap. For example, if you have Snap to Endpoint on and then move the cursor close to a
contour endpoint the cursor will snap to the point. Snapping makes it much simpler to precisely create and edit contours.

Icon Description Cursor


Snap to grid Snaps to the nearest grid point. The grid spacing is configured on the Grid page in Preferences.

Snap to guideline

Snap to intersection

Snap to endpoint

Snap to nearby contour

Snap to center of arc

Snap to midpoint

Snap to perpendicular point


Snaps to a nearby guideline when the cursor gets close. Also when dragging a contour,

 the perimeter of the contour snaps to nearby

guidelines.

Snaps to the intersection of two line  segments.

Snaps to the endpoints of arc, curve and sine  segments.

Snaps to the nearest point on a contour  when the cursor gets close to it.

Snaps to the center of an arc segment when  the cursor is placed near the arc.

Snaps to the midpoint of a segment when the  cursor gets close to it.


When constructing line segments, after defining the first point in the segment, the second endpoint will snap to a point on a contour so that the line segment will be perpendicular to the contour.

Getting Started Page 13

Snap to tangent point

Snap to tangents between two circles

Snap to show intersecting contours



When constructing line segments, the second endpoint will snap to a point on an arc so that the new line segment will be tangent to the arc.


As you move the cursor while in a construction tool, this snap identifies the tangent point on an arc segment you are near, as well as the corresponding tangent point on an adjacent arc segment. This makes it easy to construct line segments that are tangent to two arcs.


This snap toggles on/off the display of any intersecting contours in the active drawing. By identifying intersecting or overlapping contour segments, you are able to edit the drawing to fix potential toolpath creation issues before they happen.
The snap distance value, in screen pixels, is set on the General Tab of the Preferences Dialog. See
“Setting Preferences” for details.

Guidelines

Menu: View / Edit Guidelines

Guidelines are design aids that display as a dashed line in your design view. Guidelines provide a way to precisely locate points and contours in the drawing. If Snap to Guideline is enabled, contours moved near a guideline will automatically be positioned along the guideline. When working in a drawing tool, points can be precisely located either along a guideline or at the intersection of two guidelines.
 In the Edit Guidelines dialog, clicking on the Next button will allow you to move through the guidelines that have been placed. The selected guideline will be highlighted in blue and any edits will be applied to that guideline.

Edit Guidelines Dialog

Menu: View / Edit Guidelines

Use the Edit Guidelines Dialog to Create, Delete, Move, Rotate, and Lock or Hide a guideline.
To open the Guideline Dialog: Select Edit Guideline from the

View Menu.

Page 14 Getting Started

Creating a Guideline

Menu: View / Edit Guidelines

The simplest way to place a guideline is to ‘drag’ it from the horizontal or vertical rulers on the screen.
Place the guideline by left-clicking on the ruler and then dragging the guideline out into the design.
You can also create a new guideline using the Edit Guideline dialog:
1. Activate the view in which the guideline is to be placed by clicking in that view.
2. Enter in the coordinates and angle of the new guideline.
3. Click on the New button.
4. Click on Done to exit the dialog.

Deleting a Guideline

Menu: View / Edit Guidelines

1. Activate the Guidelines dialog.
2. Click on the Next button until the guideline is highlighted in blue.
3. Click on the Delete button.
 It is also possible to right-click on a guideline and then select Delete guideline from the shortcut menu. You cannot delete a guideline by dragging it out of a view.

Moving a Guideline

Menu: View / Edit Guidelines

1. Activate the Guidelines dialog.
2. Click on the Next button until the guideline is highlighted in blue.
3. Enter the coordinates for the new location.
4. Click on the Move button.

 Guidelines may also be moved interactively by simply selecting the guideline with the mouse…left click, hold and drag to the desired location. If the lock guides option has been enabled, this interactive method is not available.

Getting Started Page 15

Rotating a Guideline

Menu: View / Edit Guidelines

Activate the Guidelines dialog.
1. Click on the Next button until the guideline is highlighted in blue.
2. Enter the angle (in degrees) you would like the guideline to be rotated to in the Angle field.
3. Click Rotate.
4. Click Done.

Locking Guidelines

Menu: View / Edit Guidelines

The Lock Guidelines feature prevents guidelines from being moved or edited by accident. Guidelines may be added while the guidelines are locked, but may not be deleted, moved or edited.
1. Activate the Guidelines dialog.
2. Check the Lock Guides box.
3. Click Done.

Hiding Guidelines

Menu: View / Edit Guidelines

The Hide Guidelines feature allows you to hide the guidelines without actually deleting them. While this feature is enabled, no guidelines will be displayed, the Snap to Guidelines feature is disabled.
1. Activate the Guidelines dialog.
2. Check the Hide Guides box.
3. Click Done.

Changing the View

The commands available in the View menu and the Zoom toolbar allow you to zoom in and out to get a closer look at part of your design or see the whole thing. The zoom commands do not change the size of any part of your design; they simply change your view of the information.

Zooming with the Mouse

To zoom in and out using the mouse, hold down the CTRL key and drag with the right mouse button. Dragging the mouse up or left zooms out, down or right zooms in.

Page 16 Getting Started

Zooming using a Mouse Wheel

Zooming with a mouse wheel is a particularly handy way to get around a drawing. Move the cursor to where you want to work, and move the wheel backward to zoom out or forward to zoom in. Zooming is centered on the cursor location which makes it very easy to zoom in to a particular location.

Zoom Commands

Menu: View

Toolbar: Zoom

Function

Icon

Description

Zoom

Window

The Zoom Window command allows you to select an area to magnify.

1. Click with the mouse and drag a box around the area you want to magnify.

2. Release the left mouse button and the software will zoom in on the selected area.

Zoom In

(Ctrl + I)

Zoom in towards the center of the window.

Zoom Out

(Ctrl + K)

Zoom out and enlarge the view of the design.

Zoom to Plate (Ctrl + P)

Display the extents of the plate.

Zoom

Previous

Return to the previous zoom level.

Zoom to Extents of Selection

Zoom in on the currently selected objects. If all four views are active, all views will zoom to the extents of the selection.

Zoom to Extents of all Objects

Zoom out to display all objects, including the plate if one is designed. If all four views are active, they will all zoom to the extents of the objects in the drawing.

Redraw

Menu: View / Redraw

The Redraw Tool is used to redraw or refresh the screen and clear any remnants left over from manipulating drawing elements, from the View menu, select Redraw or press Ctrl + R.

Getting Started Page 17

View Setup Menu: View / Setup Toolbar: Setup / View Tab

The View Setup tab of the Preferences dialog determines how and what information is displayed. To
access the View Setup tab, from the View menu, select View Setup.

Undo and Redo

Menu: Edit / Undo

To undo the last operation, from the Edit menu, select Undo […] or type CTRL+Z. The name of the last operation is displayed after the Undo command.
If you decide that you didn't want to undo an action, from the Edit menu, select Redo […] or type

CTRL+SHIFT+Z

 If you have more than one drawing open, the Undo and Redo commands only affect changes made to the active drawing.

Working with Layers

Menu: Setup

Toolbar: Settings

EnRoute offers the ability to organize your drawings into Layers. Layers provide a way to separate information in the drawing so that it is possible to only display the information that you are working with at a given time. Individual layers may be displayed or hidden at any time. In addition, objects contained in different layers can be displayed in different colors to help distinguish different parts of the design.

Layers Toolbar 

Toolbar: Settings

To activate the layers toolbar click on the layers toggle icon. This will open the layers toolbar. This toolbar makes it easy to choose a particular layer to display, or to turn on all of the layers in the drawing.

By clicking on the Activate all layers icon  you can switch between the current layer displayed and displaying all of the layers.

Page 18 Getting Started

Layers Dialog

Menu: Setup

Toolbar: Settings

Each layer has several options for display and use. These options include: OnOffLock and Move

Lock. A check in the box indicates that this function is turned on for this layer.

If the Layer is:

The Objects on the layer:

On

All objects on that layer are displayed and can be selected.

Off

None of the objects on the layer are displayed, and none of the objects on that layer can be selected.

Lock

All of the objects on the layers are displayed but cannot be selected. You can still snap to the objects using the snap tools.

The current layer cannot be locked.

Move Lock

All of the objects on the layers are displayed, they can be selected but they cannot be moved.



To access the Layers dialog, click on the Layers icon

To:

Do The Following:

Select the

Current Layer

Check the box in the Current column for that layer.

The current layer is the layer in which any contours will be created.

Add a New Layer

Click New.

The layer is added to the bottom of the list, and is automatically selected as the current layer.

Delete Layers

Select the layer and click Delete.

If there are contours contained in that layer, you will be asked to confirm your action. If you delete the layer, its contents will also be deleted.

Remove Empty

Click on the Remove Empty button to remove all layers that are empty. This is useful in helping to clean up a drawing by removing empty layers.

Getting Started Page 19

Rename a Layer

Edit the text in the Name column for that layer. Highlight and type the new name.

Change the

Color of a Layer

Click on the color displayed in the Color column for that layer. A standard

Windows color selector window will open. Select the new color and click OK.

Moving Layers

To move a layer, select the layer and click on Move Up or Move Down. You can also move a layer by dragging the row header at the left edge of the list.

Hide or Display

Layers

In the On and Off column, check On to display a layer, Off to hide it. The current layer cannot be hidden.

Lock a Layer

Check the box in the Lock column to lock a layer. Contours contained in a locked layer cannot be edited or deleted.

Unlock a Layer

Clear the box in the Lock column to unlock the layer. The current layer cannot be locked.

Save Changes and Exit

Click OK to save all changes and close the dialog.

Cancel Changes

Click Cancel to close the dialog without saving any changes.

Change Layer

Menu: Transform / Change Layer

Toolbar: Settings

When an object is created, it is placed on the Current Layer. To change an object’s layer:
1. Select the objects to change.
2. Activate the Change Layer  dialog either from the menu or from the toolbar button.

Page 20 Getting Started


3. Click on the layer you want to move the selection into.
4. Click OK.

Using Help

Menu: Help

To display the EnRoute Help system, from the Help menu, select Help Contents. You can also press

F1.

Preferences

Menu: Setup / Preferences

EnRoute allows for several categories of options to be defined by the user. Access Preferences in the Setup Menu. Enter your preferred settings. Click OK to save changes. Click Cancel to close the dialog without saving changes.

Getting Started Page 21


The available settings are:

General Tab

Merge

Contours

Designs which were created and exported from other drawing programs are not always created as closed contours. This function provides for automatically merging contours together.

 

Import

Check this box to merge contours when they are imported.

 

Paste

Check this box to merge contours when they are pasted from the clipboard.

 

Tolerance

The maximum separation between contour endpoints that will still be merged.

Automatic

Cleanup

These options specify whether the program should automatically delete short segments when importing or copying contours into the program.

 

Import

Check this box to delete segments when contours are imported.

 

Paste

Check this box to delete segments when contours are pasted from the clipboard.

 

Tolerance

The maximum length of segments that will be deleted.

Undo Operations Limit

Sets the number of operations that are saved so that the Undo command can undo them.

 

Unlimited

All operations since the last save can be undone.

 

Limited

The Undo command will be able to undo only the specified number of operations.

Page 22 Getting Started

Save

The Auto Save function automatically saves the current drawing at the specified time interval.

 

Auto

Save

Check to enable the AutoSave function.

 

Time

Interval

The time interval at which the design is automatically saved.

Allow scaling of toolpath groups

After contours or reliefs have had toolpaths applied, the object is referred to as a Toolpath Group. If this is checked, it is possible to scale a selected toolpath group. When a toolpath group is scaled, its toolpaths will automatically be recalculated using the strategy parameters that were used initially. If unchecked, toolpath groups cannot be resized. Checked by default.

Clip toolpaths to plate

If checked, output toolpaths will not extend outside the boundary of the plate.

Horizontal

Cutting

If this option is available, it allows you to control whether you want to allow toolpaths to be rotated out of the horizontal x-y plane. This is only appropriate if your machine has the ability to cut toolpaths that are not in the x-y plane – most likely using an aggregate head. If this option is available in your version of EnRoute, it should most likely remain unchecked unless you specifically need to rotate toolpath groups.

Bump

Increment

Set the amount that a selection is moved when an arrow key is pressed.

 When moving a contour using the arrow keys to bump it, it is normally bumped by the increment specified here. However, by holding down the shift key, the bump becomes a portion of the display width, so it gets smaller as you Zoom In. This is a nice way to be able to bump selected objects by either a very small amount or a large amount just by changing the zoom level.

Click

Increment

Sets the amount that values in a field are changed by when the “spinner” to the

right of the field is clicked.

Snap

Threshold

The distance in pixels at which the snap function is triggered, snapping a contour to a grid point or other positioning guide.

Initialization Tab

Maximize

Application

Check this box to automatically maximize the software on startup.

Maximize

Document

Enable this function to automatically maximize new documents when they are opened.

Display 4 Views

Check to display designs in the 4-view mode by default.

Prompt for Plate

Check to open the Define Plate dialog automatically when a new design.

Small Part Size

Threshold

This parameter is used by EnRoute for selecting ‘small parts’ when the option to

output small parts first is selected in the output dialog.

Getting Started Page 23

Solutions Path This defines the path of any installed 3rd party applications that provide additional functionality to EnRoute.

Display Tab

The Display tab allows the user to define which colors are associated with the different types of drawing elements.
To change a color:
1. Double-click on the color you want to change.
2. Select the color desired and click OK.
3. Click OK to exit and save any changes.

Show Layer

Colors

Check this box to show the colors assigned to the individual layers.

Update

Buttons

This should typically be checked. It allows EnRoute to update buttons so that buttons are only enabled when they are appropriate based on the current status of the selected objects. If it is not checked, then buttons will be left enabled even though they might not be functional.

Real-time rendered panning

EnRoute offers the ability to have full-time rendered move-pan-rotate of reliefs in the perspective view, allowing users to spin their designs around to better understand how they will look when completed. If real-time panning for some reason causes a problem with your computer, it is possible to disable this feature by changing a parameter in EnRoute’s preferences configuration file. If you feel this is necessary, please contact EnRoute Technical Support for assistance.

Rendering Options – Choose the option that best fits your hardware configuration.

OpenGL Level 3

This is the most advanced option. It uses the graphics card on your computer to perform OpenGL rendering in the perspective view.

OpenGL Level 2

This is the option that was the default method in EnRoute 4. Some users may continue to find this to be the preferable rendering method for their computer configuration.

OpenGL Level 1

This option has proven to work best on computers that do not include a dedicated graphics card for rendering, instead relying on a graphics chipset on the computer motherboard.

Windows Graphics

If your computer does not have OpenGL rendering capabilities, this method of rendering will still provide good results but will not be quite as fast.

Page 24 Getting Started

Units Tab

The Units tab allows you to select the units that will be used to measure LengthTime and Speed in the software.
If the units are changed while a drawing is open, the size of any existing objects will be converted to the new units so that they remain the same size.

 If the units are changed while a design containing toolpaths is open, the measurements of the toolpaths may not be converted correctly. For this reason, you should save and close the drawing, then change the units and reopen the drawing. This ensures the toolpaths will be converted properly.

Grid Tab

The Grid tab allows the user to determine the view of the grid shown on the document page. Using the grid can be helpful in determining the placement of objects. There are two levels of the grid that may be enabled and adjusted to the layout of a particular project.

Show Grid

A checkmark in this box indicates the grid is turned on.

Interval of the grid marks

The distance between the grid marks.

Style of grid marks

Select NoneCrossTick, or Line.

Size

Size of the grid marks in pixels.

Color

Color of the grid marks.

Show grid in perspective

Check this box to display the grid in the Perspective view.

View Setup Tab

The View Setup tab determines how information is displayed on screen.

Standard Items

Plate

Check this box to display the plate, if any.

Contours

Check this box to display the contours.

 Since contours are the main type of drawing element, this is typically left on. Sometimes it can be convenient to turn contour display off to review only the toolpaths.

Contour Loops

Check this box to display contour loop indicators. EnRoute checks selected contours for loops before attempting to create toolpaths. If loops are detected, and you choose not to proceed with the toolpath operation, the points at which the contour crosses itself will be indicated with contour loop indicators. If you do proceed with the toolpath operation, EnRoute will remove the loops automatically. In some instances, this might modify the contour in a way that you did not intend.


Getting Started Page 25

Open Contour

Direction

Check to display direction arrows on open contours.

Popup menu on Right Click

Check to enable a right click with the mouse to bring up a popup menu for the tool you are using.

Toolpath Items

Toolpaths

Check this box to display the toolpaths.

Direction

Check this box to display direction arrows on toolpaths.

Entry/Exit

Check this box and the Start Point to display the Entry/Exit positions for each toolpath.

Bridges

Check this box to display the location of toolpath bridges.

Start

Point

Check this box to display a small circle with an X in the middle at the start point of each toolpath. If you want to see the Entry/Exit toolpaths make sure the Start Point is turned on also.

Toolpath

Width

The Width option determines how toolpaths are displayed on screen. There are two options:

 

Lines

The toolpaths are displayed as lines with directional arrows (Default).

 

By

Tool

The toolpaths are displayed using the diameter of the tool used to create the toolpath.

 This option will give you a better idea of what the final piece will look like after it has been machined. The Simulate 2D command located in the Machining Menu will show the same thing as the By Tool option, in addition to showing the cutting sequence.

 It is easy to toggle this display mode by using the F9 key.

Depth

This option controls how the depth of the toolpaths affects the way they are displayed.

 

All

Depths

All toolpaths at all depths are displayed (Default).

 

Surface

The toolpaths at the surface is displayed.

 

Final

The last (bottom) toolpath is displayed.

 

[Specific depth]

One of the specific depths assigned to the passes is selected for display.

Tools

This option selects which toolpaths will be displayed based on the type of tool associated with the toolpath. The options displayed are based on the tools used in the active drawing.

 

All Tools

Toolpaths for all tool types are displayed (Default).

 

[Specific

Type]

Only the toolpaths which use the selected type of tool are displayed.

Page 26 Getting Started

Relief Tab

Toolpath

Tolerance

This parameter defines how closely 3D toolpaths follow their relief. This value might vary depending on the size and resolution of the reliefs. The smaller the tolerance the more closely the toolpaths will follow the relief, but this will also create more segments in the toolpaths and increase the size of the output files.

Relief

Lighting

You can adjust the lighting of the relief with these parameters.

Start Points

This tab allows you to define a preference for where start points are automatically located on Routing
Offset toolpaths.

Long Edge and Edge Midpoint

This will locate the start point on the longest edge of the contour. If Edge Midpoint is checked, then the start point will be moved from the start of the long edge to its midpoint.

Direction

This option allows you to define a direction that EnRoute will then use to locate the start point. The direction is entered in the edit box to the right in degrees, relative to the origin of the drawing.

Magnetic

This option allows you to enter a specific point, and then EnRoute will create the start point for each object as close to that point as it can. This allows you to automatically pull start points toward an area of the material.

Longest

Segment

This option picks the longest segment within the contour and locates the start point either at the start or the midpoint of the segment depending on whether the Segment Midpoint option is checked.

Dimensions Tab

The Dimensions Tab sets up the display parameters of the dimension tools. All dimensions in the drawing will be displayed using these parameters.
Text Select the font for the dimension text.

Getting Started Page 27

 This parameter sets the height of the text in the dimensions tool.


This parameter sets the distance that the extension lines start to draw from the start and end points of the dimension.

 This parameter determines the height of the arrow.  This parameter determines the width of the arrow.
This parameter sets the number of decimal positions for the measurement of a line
segment.
 This parameter sets the number of decimal positions for the measurement of an angle.  This sets the position of the text above the arrow line.

 This sets the position of the text in the center of the arrow line.


This sets the position of the text under the arrow line.

Ordering Tab

The Ordering tab allows you to define default ordering preferences so that when toolpaths are automatically ordered by EnRoute, the order will follow your preferences. The layout of this dialog is essentially the same as the ordering dialog that is presented in other tools such as Output, 2D Simulate, Ortho Simulate, and the Rendering tool. And, they are all related.
It is possible from each of those other ordering tools to reset the ordering to match these preferences, and it is also possible to send the current ordering settings in a file to the ordering preferences. For example, maybe you have defined your preferences so that Routing Offset strategies come before Drill strategies. And then you find that when you prepare your jobs for output you always change the Strategy Order so that the routing offsets go last. From within the output dialog you can easily make those updated choices become your ordering preferences. Then the next time you create a design that includes routing offsets and drills, the default ordering settings will reflect the updated preferences that have the routing offset after the drills.

Page 28 Getting Started


The following table provides a brief
description of each of the parameters in the
Ordering Preferences dialog.

Priority

Order

Set the priority order for the order in which toolpaths sorted. In the priority settings in the graphic above, the toolpaths will be sorted based on the Tool Order as the top priority, followed by the Object Order, Strategy Order, etc... A more detailed explanation of the ordering philosophy in EnRoute is located in Chapter 11 of this manual.

Tool Order

You can choose tools from EnRoute’s tool library to add to the Tool Order list. You might typically add tools that you use often, and then click and drag them into the preferred order.

Strategy

Order

This list includes all of the strategy types available in EnRoute. By default they are in a reasonable order – drills are first in the list and routing offsets are last. You can click and drag these strategy types into your preferred order.

Object Order

You can choose the default object ordering method, including shortest, rows, columns, inside out, and outside in.

Small Parts

First

If this is checked, objects with a surface area less than the small part size

threshold defined in the Initialization tab will be put at the top of the object order list regardless of the object ordering method.

Maintain

Grouping

If objects are grouped together, this checkbox allows them to be treated as one object for object ordering.

Add Tool

This button allows you to add a tool to the Tool Order list.

Delete Tool

This button removes the current tool from the Tool Order list.

Clear Tools

This button clears all the tools from the Tool Order list.

Reset Active

This resets the currently active parameters (Priority, Tool, Strategy or Object) to their default values.

Reset

Parameters

This resets all the ordering parameters to their default values.

Getting Started Page 29

Exiting the Software

Menu: File

From the File menu, select the Exit command to close all layouts and exit the program.

Page 30 Getting Started

3. Toolbars and Command Icons


This section provides a summary of the major functions of EnRoute. As you will recognize, most of the commonly used tools are readily available by clicking the screen buttons available in the toolbars. The icons presented and described in this section are organized based on the toolbars in which they reside.
The toolbars can easily be moved to the top, bottom, right or left side of the display. This allows you to customize the interface to fit your preferences. The changes you make will be saved when you exit so that the layout will come back just as you left it the next time you start the program.
Until you become familiar with each of the icons, you can view a short “hint” about each icon by placing
the cursor over the button and leaving it there for a second or two.
In addition to the screen icons, you can also reach all of the EnRoute functions by using the pull down menus.

File Toolbar


New (Ctrl+N) - Use the New command to start a new drawing. EnRoute supports the

 Multi Document Interface (MDI), which allows you to have more than one layout open at a time.

Open (Ctrl+O) - Use the Open command to open an existing EnRoute file. When you open a file it is placed in its own drawing window, not the current one.

Import a File - Use the Import command to load a file that has been saved in a compatible format other than the native EnRoute format.

Save (Ctrl+S) - Use the Save command to save the current design file. If you are saving a file for the first time, the Save File As dialog will be displayed.


Print – The Print command gives you the opportunity to print the current screen view or drawing.

 Calculator - This will activate the windows calculator tool.


Save Snapshot of Active View – This tool allows you to take a snapshop of the active view and save it to a file.

Measure Lengths- This tool opens a toolbar with access to several measurement tools.

Cut (Ctrl+X) – The Cut command allows you to remove items from the design file and

 place them in the Windows Clipboard so they can be “pasted” either back in the original

file, or in another design file.

Toolbars and Command Icons Page 31

Copy (Ctrl+C) – The Copy command is similar to the cut command, except it places a copy of the selection into the clipboard.

Paste (Ctrl+V) – The Paste command takes information that is stored in the Windows

Clipboard and places it in the currently active design file.

Delete – Use this tool to delete the selected objects.

Undo (Ctrl+Z) - Use the Undo command to reverse your most recent actions. The Undo command may be chosen as many times as needed to undo previous editing operations

 up to the first operation in the editing session. If you load a file and make a number of editing changes to it, EnRoute will allow you to Undo all of the changes.

Redo (Shift+Ctrl+Z) Redo command to reverse any operation changed by the Undo

 command. You can continue to select the Redo command until all of the Undo operations have been reversed.

Zoom Toolbar


Zoom Window – Use the Zoom Window command to magnify a selected area. The Zoom

 Window command is different than the Zoom Out and Zoom In commands in that you can specify a particular area for the zoom to cover.

Zoom In (Ctrl+I) - Use the Zoom In command to zoom up or magnify the current window.

Zoom Out (Ctrl+K) - Use the Zoom Out command to zoom straight back.


Zoom to Plate (Ctrl+P) – Use the Zoom to Plate command to magnify to the extent of the plate size.

Zoom Previous - This command will return you to the previous zoom display.


Zoom to Extents of Selection - Use the Zoom Selection command to display the selected group in the current layout.

Zoom to Extents of all Objects– Use the Zoom to the Extents command to display all design objects in the current file. This will include the plate if one is defined.


Page 32 Toolbars and Command Icons

Settings Toolbar


Define Layers (F7) – This icon activates a dialog that allows the user to

 manage the layers that are used to store drawing elements. Within this dialog you can specify the active layer.

Change Layers – Activates a dialog that allows you to change the layer to store the current selection.

Toggle the layers toolbar – Opens or closes the layers toolbar.

Toggle the snaps toolbar – Opens or closes the snaps toolbar.

Precision Input Tool – Opens the Precision Input Dialog.

Libraries Toolbar



Redefine the Current Plate – This activates the dialog to define the plate in the current drawing. The Plate provides a good reference during the design process and it also provides a means of making sure that toolpaths stay within the limits of the material you are using.


Create Plate from Selected Contour – This tool allows the user to select a  contour shape to be used as the plate. This allows for the easy use of remnant
materials.

Define Plate Panels for Oversized Designs- (Ctrl+Alt+P) – This tool allows you to define a specific area of the plate that you want to output the toolpaths for. It helps if you have a large design that is larger than your machine’s table size, or larger than the material you have available.


Material Library (F4) – The Material Library provides a method for customizing settings for your machine and specific activities. You may define speeds for different types of materials (wood, metal, etc.) that are to be routed or

engraved. When the Define Plate command is used, there is the option to
select a material type to be associated to the plate. Speed settings can be set for the materials you use most often so that EnRoute will apply these parameters to new toolpath strategies jobs without having to re-specify them each time.

Toolbars and Command Icons Page 33


Tool Library (F5) - The Tool Library command is used to define routing and  engraving tools used with the toolpath commands. The tool geometry
entered for each tool is used to generate toolpaths.

Driver Setup (F6) - This icon will bring up the parameters for the currently active driver. Each driver parameter may be edited and then saved back to the driver configuration file. All of the drivers that have been installed on the computer are available to be selected as the active driver.

Output Toolbar



Generate Output - This is the main icon used to send toolpath output either to a file or directly to the machine. In this dialog the user defines how the information is to be sent, how the toolpaths are ordered as they are output, and which toolpaths are included.

Automatic Toolpath - The EnRoute Wood version of EnRoute provides

 Automatic Toolpath (ATP) capabilities that allow you to process parts contained in external DXF geometry files.

Simulate 2D (F8) – This icon activates a mode in which the user can visualize how the toolpaths will be sent to the machine. The toolpaths are drawn to the

screen in the same sequence that they will be sent to the machine as output.  Statistics regarding the number of tool changes and the number of tool lifts are
also presented in this mode. In addition, the user has the opportunity to modify
the order of the toolpaths and then immediately see the effect on the output using the 2D simulation.

Simulate Ortho - This icon activates a mode similar to the 2D Simulation except it is in the perspective view. The toolpaths are drawn to the screen in the same

sequence that they will be sent to the machine as output. Statistics regarding  the number of tool changes and the number of tool lifts are also presented in
this mode. In addition, the user has the opportunity to modify the order of the
toolpaths and then immediately see the effect on the output using the Simulate
Ortho mode.

3D Rendered View - This icon activates a 3D mode that allows you to view a  solid model of your material, and the results of the toolpaths cutting the
material. This mode is useful for seeing the effects of both 2D and 3D toolpaths.

Project Toolpaths - This tool provides a method for tipping toolpaths

 vertically. It is useful for cutting non-horizontal surfaces, and is likely most useful for routing offset and fills.


Set Toolpath Order – This tool is used to manually set the order of the objects as they will be used to generate output. The user can define the order using different methods for sorting the objects or define the specific order by selecting the sequence with this tool.

Page 34 Toolbars and Command Icons

Object Edit Toolbar



Selection Tool – This is the main selection tool in EnRoute for selecting, rotating and scaling objects.

Move Tool (Shift + F5) – This tool allows the user to precisely move an object.

Scale (Shift + F6) – This tool is used to precisely scale objects. By selecting a group of  objects and then clicking on the scale icon the user can enter precise size or scale

information to change the size of the selection.

Rotate (Shift + F7) – This tool is used to either interactively or precisely rotate selected objects.

Mirror Object (Shift + F8) - This tool is used to interactively mirror an object.



Group (Ctrl+G) – This command is used to group two or more objects together so they may be selected and manipulated as a unit. After the objects have been placed in a group, they can be selected as a group by clicking on any member of the group. Also, they may be released to return them to their original state as separate objects.

Ungroup (Ctrl+U) – This command is used to release objects from a group to their original state as separate objects.


Alignment – This icon can be used to activate a toolbar that presents a number of different options for aligning the objects in a selection. The first icon is used to align objects to center both horizontally and vertically. The additional icons in this toolbar provide other alignment options.


Weld –This icon is used to activate a toolbar that presents a number of options for welding selected objects. The first icon is used to weld objects that are overlapping each other into one single object. Additional options include: Weld Common and Weld Subtract, as well

as two interactive welding tools.

Nest - This tool allows you to arrange selected objects into the plate in a configuration that will allow them to be cut out so they will efficiently utilize the material. Select the objects

 you want to nest and then click on the Nest icon. This will activate a dialog for specifying

nesting options and parameters. This icon is also used to activate a toolbar that contains
two additional tools, Dynamic Nesting and Nesting Report.

Toolbars and Command Icons Page 35

Toolpaths Toolbar



Edit Toolpath Plan – This icon activates the Plan dialog that allows you to edit  the Plan associated with the selected toolpath groups. The Plan represents the
strategies applied to a toolpath group.

Routing Offset – The Routing Offset command is used to offset, or compensate, for the engraving or routing tool. This will make sure no matter what size tool you use the parts will be the correct size. You can also use this command to create inlayed objects. Click and hold to open the flyout menu.

Kerf Compensation – This tool creates offset toolpaths that are much like routing offsets, except that they are intended to be used with other types of cutting, such

 as plasma, water jet or laser cutting. The interface is simplified, and it is also

possible to add loops to the corners so that the cutter does not decelerate as it

approaches an external corner on a part.

Daisy Chain - This tool can be more efficient because it allows the cutting to be done without having to lift the tool out of the material as often.

Hatch Fill – The Hatch Fill command is used to generate a series of toolpaths to remove an area or section of material.

Island Fill – The Island Fill option is a series of inlines (lines and arcs) that are generated until the selected contours are filled.

Drill - The drill functions provide tools for adding drill objects to the design. Drill objects are a special type of toolpath group that define drill points that can either

 be created on their own, or be created based on selected contours. Drill points

can be created in patterns such as arrays, around a circle, and along a path.

Multiple tools can be specified for any drill point.

Slot – The Slot command is used to create a single line that the router will cut.

Engrave – The Engrave command is used to generate a machine path on the original contour to be engraved or to generate a 3D path without a fill.




Pyramid – This type of toolpath strategy is used to create a positive bevel on the selected set of contours using a conic-shaped tool. It can also include a roughing pass to ensure that the pyramid tool will be able to complete its cuts, and an offset toolpath to cut the pieces out after the beveled tool has completed its work. This method is popular for making lettering and artwork that is commonly referred to as beveled, chiseled, sculpted, or prismatic.

Delete Toolpath – This command allows the user to delete toolpaths that have been applied to selected objects.


Page 36 Toolbars and Command Icons

Contour Editing Toolbar



Edit Points - This tool provides access to a number of editing functions. You can move, insert, and delete points, open and close contours, change segments to arcs, curves and lines. After selecting the tool and clicking on a contour, right click to make these functions available.


Extend/Trim - The Extend tool is used to extend an open contour either interactively, by a  specific distance, or to intersection with another contour segment. If you click and hold
this button, a flyout menu will open. From there you can access the Trim tool.


Fillet Corners – This tool provides a method to insert rounded corners, or fillets, at selected corners in a contour.

Join Contours - This tool allows you to connect open contours at their endpoints either into an open or closed contour.

Offset Contours - This tool opens a dialog that allows you to enter parameters to offset a closed or an open contour.


Multicopy – This tool opens a dialog which allows you to produce multicopies of an object in three different ways.


Vectorize Bitmap - This powerful tool is used to create a series of closed vector contours from a bitmap image. In order to create toolpaths in EnRoute, it is necessary for the artwork to be represented by vectors. This tool provides the means of converting scanned images or other bitmap images into vectors so that they may be used to create toolpaths.


Cleanup Contours - When bitmap images are vectorized, the vectors often require some degree of ‘cleaning up’ in order for them to be appropriate to toolpath. This tool provides an automated means of cleaning up contours, by reducing the number of curve segments to create smooth contours that will then create better toolpaths.

Construction Toolbar



Draw Polyarc – This tool is used to create a series of connected line or arc  segments that can either be open or closed. Click and hold to activate a flyout
toolbar that contains a number of other line drawing tools.

Draw Rectangle – This tool will open the Precision Toolbar for the rectangle. Rectangles can be precisely or interactively created.

Toolbars and Command Icons Page 37


Draw Circle – This icon activates the Precision Toolbar for the circle. Several tools are available to interactively or precisely create a circle.


Draw Ellipse – This tool will open the Precision Toolbar for the ellipse. Create an ellipse interactively or precisely.



Draw Arc – This tool activates the Precision Toolbar that provides other arc construction options.

Component Creator - This tool is a quick an easy way to create slotted components that can be both decorative and structural.

Draw Polygon – This button activates a dialog for defining the parameters for placing polygon shapes.

Text – This tool opens a Precision Toolbar. Any True Type® font that is

 installed on your computer is available to be used. The toolbar allows for many options in placing and editing the text to create the desired effects.


Shape Wizard – Click and hold to open a toolbar containing the Shape Wizard  tools. These tools provide several different methods for creating shapes using

parameters to define size and shape.

Create Dimensions – Click and hold to open a set of dimension tools to be used to measure and record in the drawing.

3D Surfaces Toolbar




Create Relief - This icon opens a dialog that enables several options to create a relief for the selected contours.

Edit Selected Relief – This icon opens a dialog that provides several relief editing tools that allow the user to interactively edit a selected relief.



Textures – Click and hold this icon to open a flyout menu containing several different textures that can be edited and applied to a relief.

Symmetric Parametric Textures – Click and hold this icon to open a flyout menu containing several different symmetric textures that can be edited and applied to a relief.

 Rapid Texture – This opens a tool designed to create textured panels using the diameter of the tool to create the texture.


Extrusions - This icon activates a toolbar that provides additional options in creating  reliefs. These tools use revolutions and extrusions to create meshed objects and modify

selected relief surfaces.

Chamfer - This icon activates a toolbar allowing the selection of different chamfering tools. The Chamfer tools allow you to modify reliefs by applying profiles that can range


Page 38 Toolbars and Command Icons



anywhere from a simple rounded edge all the way to an intricate profile that changes the whole relief.

Apply Mesh - This icon activates a dialog designed for the application of 3D meshes to reliefs. Meshes are made up of triangles of varying sizes that define their surface.

Slice Mesh - This tool allows you to create 2D ‘slices’ of a selected mesh model that can then be stacked to create a representation of the model.

Apply Bitmap - This icon enables a dialog used to apply bitmap images as a method for  modifying relief surfaces. The application method defines how the bitmap will be applied
to the relief surface.

Merge Reliefs - This tool allows you to merge one or more reliefs with a base relief. This  allows you to create portions of a relief separately and then merge them together to

create the final surface.

Smooth Relief – Click and hold this icon to activate a toolbar that provides tool options that allow you to modify reliefs to fit the needs of your design.


Align Reliefs - This icon can be used to activate a toolbar that presents a number of different options for aligning the reliefs in a selection. The first icon is used to align all reliefs to the bottom of the plate. The additional icons in this toolbar provide other alignment options.

Create Primitive Objects - The Primitives tool is used to create a range of basic 3D

 mesh shapes. These shapes can be used to build more complex shapes, or they can be used as design elements in your relief.

Rendered View - This icon activates a rendered view of the selected relief.

Delete Relief - Deletes the selected relief.

Snaps Toolbar


Snap to grid – Snaps to the nearest grid point. The grid spacing is configured on the Grid page in Preferences.

Snap to guideline – Snaps to a nearby guideline when the cursor gets close. Also when dragging an object, the perimeter of the object snaps to nearby guidelines.

Snap to intersection – Snaps to the intersection of two line segments.

Snap to endpoint – Snaps to the endpoints of arc, curve and sine segments.



Toolbars and Command Icons Page 39

Snap to nearby contour – Snaps to the nearest point on a contour when the cursor gets close to it.

Snap to center of arc – Snaps to the center of an arc segment when the cursor is placed near the arc.


Snap to midpoint – Snaps to the midpoint of a segment when the cursor gets close to it.

Snap to perpendicular point – When constructing line segments, after defining the first  point in the segment, the second endpoint will snap to a point on a contour so that the line
segment will be perpendicular to the contour.

Snap to tangent point – When constructing line segments, the second endpoint will snap to a point on an arc so that the new line segment will be tangent to the arc.

Snap to tangent between two arcs – This snap identifies two tangent points between two  arcs, when the cursor is placed near one of the tangents. This makes it easy to construct
lines that are tangent to two circles or circular arcs.

Show Intersecting Contours – This toggle shows all of the points in the drawing where  contours intersect. This is a good way to be able to see potential problem areas for
toolpathing, such as overlapping segments or intersecting contours.

Routing Offset Toolbar



Routing Offset – The Routing Offset command is used to offset, or compensate for, the  engraving or routing tool. This will make sure no matter what size tool you use; the parts
will be the correct size.

Routing Offset Open Contour - This command is similar to the standard routing offset tool  except that it is used for open contours instead of closed contours. This imposes some
limitations on the types of offsets that make sense with an open contour.

Drill Toolbar


Drill Point - The Drill Point command is used to create a single hole or pierce point.


Drill Circle - The Drill Circle command is used to create a pattern of drill points around the radius of a circle.


Page 40 Toolbars and Command Icons


Drill Array - The Drill Matrix command is used to create a series of drill points by rows and columns to form a grid.


Drill Center of Objects -The Drill Centers command is used to place a drill point in the center of the selected contours.


Drill Along Contour - The Drill Contours command is used to create a series of drill points along a contour.


Drill Corners of Plate - The Drill Corners command is used to create a pattern of drill points around a Plate. You must have defined a plate before you can use this command.

Alignment Toolbar


Align Bottom – Use this command to align the bottom of objects that have been selected.

Align Top – Use this command to align the top of objects that have been selected.

Align Centers Vertical - Use this command to align the vertical centers of selected objects.



Align Centers Horizontal – Use this command to align the horizontal centers of selected objects.

Align Left – Use this command to align selected objects to the left side.

Align Right – Use this command to align selected objects to the right side.


Weld Toolbar



Weld Joined – This is the most commonly used method for welding objects. It works by  combining overlapping objects into one object by creating a new object that is defined by
the outer perimeter of the overlapping objects.

Weld Common – This tool is used to define a new object based on overlapping

 contours. The new contour is defined by the perimeter of the overlapping portion of the contours.


Toolbars and Command Icons Page 41


Weld Subtract – Weld Subtract subtracts from the object that was selected first, using all subsequently selected objects.


Jigsaw Weld - This is a design tool used to create a shape in which both open and closed contours may be used in the creation process. It is an interactive tool. By moving the cursor into different areas on the screen, EnRoute looks for closed shapes that can be formed by overlapping contours.


Cut by Line – The Cut by Line tool allows the user to “cut” an object with a line drawn

across it to make two separate objects.

Extrusions Toolbar



Revolve to create surface - The Revolve tool allows you to use one or more contours to revolve around an axis to either modify a relief or to create a new mesh object.


Spin Contours - With the Spin tool the selected contours are spun around the Z-axis, located at a center of rotation that is defined by the user.


Extrude Contours - The Extrude tool provides a means to extrude a profile along a path to either modify a relief or create a mesh object.


Sweep Two Rails - The Sweep Two Rails tool provides another method of using profile contours to either modify an existing relief or create a new mesh surface.

Chamfer Toolbar



Chamfer Relief - The Standard Chamfer works by first adding a height to a relief that is  equal to the height of the profile, and then removing material around the perimeter of the
relief in the shape of the profile.

Chamfer Centerline - The Chamfer Centerline tool creates a chamfered surface using a profile where the profile size is modified so that it extends to the centerline of the shape.


Baroque Chamfer - This tool allows the user to simulate the effects of a traditional hand-  carved surface. It automatically determines convex and concave sections of the artwork
and then applies different profiles to these sections with smooth transitions between them.

Page 42 Toolbars and Command Icons

Mesh Toolbar



Slice Mesh - This tool allows you to create 2D ‘slices’ of a selected mesh model that can

then be stacked to create a representation of the model.

 Unwrap Mesh onto Relief – This tool is used to unwrap the mesh onto a relief.

Align Reliefs Toolbar



Align all reliefs to bottom of plate - Aligns each of the selected reliefs to the bottom of the plate.


Align selected reliefs to bottom of plate - Aligns the selection to the bottom of the plate. The relative position of the reliefs in the selection doesn’t change.


Align all reliefs to top of plate - Aligns each of the selected reliefs to the top of the plate.


Align selected relief to top of plate - Aligns the selection to the top of the plate. The

relative position of the reliefs in the selection doesn’t change.

Align all reliefs to center of plate - Aligns each of the selected reliefs to the middle of the plate.


Align selected reliefs to center of plate - Aligns the selection to the middle of the plate. The relative position of the reliefs in the selection doesn’t change.


Align relief contours to top of plate – Aligns the contours that contain the relief to the top of the plate. This is the default location for reliefs before they are moved vertically.

Modify Relief Toolbar



Smooth Relief - This tool allows you to be able to soften, or smooth, the relief either to make it more attractive or to make it so that it will machine better.


Toolbars and Command Icons Page 43

Invert Relief - This is a simple way to convert a 'positive’ relief to a ‘negative’ relief.


Fit Relief to Plate - This tool will automatically position and scale a relief so that it fits vertically within the defined plate in your active drawing.


Apply Draft angle to Relief - This function allows you to add a draft angle to your relief.  This is a slight angle between core and tool to aid the withdrawal of the product from a
mold.

Create a Mesh surface from Relief - This tool allows for the creation of a mesh surface from a relief.

Offset Relief Surface - Offsetting a relief surface can enhance EnRoute’s applications

 for mold-making. It is also an interesting creative tool, and can be used to improve the effects achieved with Rapid Texture.

Dimension Toolbar




Single Dimension – This tool allows you to determine the dimension between two selected points.

Angle Dimension – This tool allows you to determine the angle of two selected points.

Radius Dimension – This tool allows you to determine the radius of a selected circle.

Diameter Dimension – This tool will determine the diameter of a selected contour.



Leader Dimension – This tool allows you to place a leader arrow in the selected location of the drawing.

Relief Toolbar


Merge Reliefs – This tool is used to merge one relief to another.

Combine Selected Reliefs – This tool will combine two or more selected reliefs.



Extract a slice from a relief – This tool allows for a section of the relief to be extracted from the relief.


Page 44 Toolbars and Command Icons

Nest Toolbar



Nest– This tool is used to automatically nest the objects on the plate according to selected parameters.


Dynamic Nest – This tool allows the user to specifically place the objects on the plate.

Nest Report– This tool will activate a detailed nesting report that is displayed using your default browser.

Scale Toolbar


Scale – This tool is use to interactively scale an object.

Distort – This tool lets you stretch an object disproportionately.


Patch Distort – This tool allows selected objects, both contours and reliefs, to be distorted by defining the shape of a container for the selected objects.


Add Noise to Objects - This tool allows the user to parametrically distort selected contours and reliefs in order to introduce affects ranging from subtle to dramatic.

Fill Toolbar


Island Fill – This tool is used to create Island Fill toolpaths.

Spiral Fill – This tool is used to create toolpaths in a spiral pattern.



Toolbars and Command Icons Page 45

Draw Lines Toolbar


Draw Line – This tool is used to draw a line between two specific points.


Draw Polyarc - The new Polyarc tool allows you to construct a series of lines and arcs  to form a new contour.

Draw Bezier Curve – This tool allows you to draw precisely curved lines.

Sketch – This tool allows you to “freehand” sketch a curved contour by holding down the clicking and holding the left mouse button and moving the mouse to draw the

 contour. When you release the mouse button, EnRoute creates smoothed curves

through the path you have identified. If you place the mouse back near the start point
when you release the mouse button, a closed contour will be created.

Geometry Creation Wizards


Box Wizard – Design and create boxes to assemble.

Boxter Wizard – Create cabinets with this tool.



 Cone Wizard – Easy tool to create cone shapes.

Cowboy Wizard – The shape of a cowboy is preloaded.


Cut Off Corners Wizard- This tool helps to quickly calculate and cut corners of a rectangle shape.


Flange Wizard – Create a circular flange shape, including a center hole and a bolt hole pattern.

Fleur De Lis Wizard – Preloaded Fleur De Lis shape.

GCode Wizard – This tool allows you to open a G-Code output file and import it into

 EnRoute. This is one way to verify that an output file was created correctly, allowing you to evaluate it in an EnRoute drawing.


Page 46 Toolbars and Command Icons

Gusset Wizard – Create a gusset shape.

Lift Lug Wizard – Create a standard shape with a rounded top and center hole.


Lift Lug Wizard 2 – Create a standard shape with a rounded top and center hole and tapered sides.



Part Round Wizard – This tool can help to calculate and create a partial portion of a designated round part.

Corner Round Wizard- Another rounded part.

Thread Pitch Wizard – This creates a circular spiral path that can be toolpathed using an Engrave strategy and used with a thread cutting tool to cut threads in a part.

Extend/Trim Toolbar



Extend Contour –This tool is used to extend an open contour either interactively, by a specific distance, or to and intersection with another contour segment.


Trim Contour – This tool allows you to shorten a contour either interactively, by a specific distance, or based on intersections with boundary contours.

Edit Contours Toolbar


Edit Points – This tool allows you to manipulate line, curves and points in contours.


Linearize Curve Section - This tool allows you to edit a contour to define line segments between two points.


Insert Corner – This tool allows you to interactively place a corner in an existing contour.


Smooth Approximation Tool – This tool allows you to interactively edit a contour to smooth the segment between two selected points.


Add Noise to Objects- This tool allows the user to parametrically distort selected contours and reliefs in order to introduce affects ranging from subtle to dramatic.


Toolbars and Command Icons Page 47

Offset Toolbar



Offset Closed Contour – This tool allows you to define one or more offsets to a selected closed contour.



Offset Open Contour – This tool allows you to create offsets for selected open contours.

Text Toolbar


Create New Text Objects – This tool is used to interactively create text objects.

Edit Existing Text Objects – Use this tool to edit existing text objects.

Convert Text Objects to Curves – This tool converts the text objects to curves so that you can then apply toolpaths.

Textures Toolbar



Bamboo Texture - This texture creates the look of Bamboo, providing control over the joint spacing, diameter, texture, and spacing of the bamboo stems.

Basic Noise Texture – This texture creates a bumpy surface using just a power parameter and the scale of the texture.

Brick Texture – This is a simple Bricks and Mortar texture that can be applied to reliefs.

Cellular Texture – Cellular Texture breaks up space into cells or regions.



Page 48 Toolbars and Command Icons

Dot Texture – Dots Texture will give a variety of textures based on circles.



Flagstone Texture – Flagstone texture simulates a mosaic of stone tiles. The stones appear to be selected to fit together but have a random grain direction.

Flame Texture – Flames texture simulates the look of flames.

Flow Texture – This is texture that creates a nice flowing look.

Hammered Texture – This texture can create many different looks of textures.

Hexes Texture – Hexes texture produces a hexagonal or honeycomb pattern.

Marble Texture – Marble texture produces a pattern of veins in the relief.

Mudpot Texture – The Mudpot texture basically looks like the surface of bubbling mud.

MultiCell Texture – The MultiCell texture is related to the cellular texture but with more control parameters. Cellular texture breaks up space into cells or regions. The point being evaluated falls into one cell. The texture calculates the distance to the center of that cell and centers of adjoining cells. Combining these distances gives different effects.

MultiFract Texture – MultiFract texture can be generally described as a roughness texture. Adjusting the parameters will change the appearance of the texture in a wide variety of ways.

Phase Texture – Phase texture creates more of a flowing type of texture.

Terrain Texture – Terrain texture gives options to create the look of the landscape.



Veneer Texture – Veneer texture like the Wood texture simulates the look of wood rings and grain in the relief. The veneer produces a series of slices through the wood and tiles them next to each other.

Weave Texture – Weave texture produces a simple basket weave or textile pattern in the relief.

Wood Texture – Wood texture simulates the look of wood rings and grain in the relief. The appearance of different species of wood can be simulated by adjusting the various parameters of the texture.


Toolbars and Command Icons Page 49

Symmetric Parametric Textures Toolbar


Basic Noise2 Texture – This texture creates a bumpy surface using just a power parameter and the scale of the texture.



Bricks2 Texture – This is a simple Bricks and Mortar texture that can be applied to reliefs.

Cellular2 Texture – Cellular Texture breaks up space into cells or regions.

Dots2 Texture – Dots Texture will give a variety of textures based on circles.

Flagstone2 Texture – Flagstone texture simulates a mosaic of stone tiles. The stones appear to be selected to fit together but have a random grain direction.

Flow2 Texture – This is texture that creates a nice flowing look.

Hexes2 Texture – Hexes texture produces a hexagonal or honeycomb pattern.

 Mudpot2 Texture – The Mudpot texture basically looks like the surface of bubbling mud.



MultiCell2 Texture – The MultiCell texture is related to the cellular texture but with more control parameters. Cellular texture breaks up space into cells or regions. The point being evaluated falls into one cell. The texture calculates the distance to the center of that cell and centers of adjoining cells. Combining these distances gives different effects.

MultiFract2 Texture – MultiFract texture can be generally described as a roughness texture. Adjusting the parameters will change the appearance of the texture in a wide variety of ways.


 Phase2 Texture – Phase texture creates more a flowing type of texture.

Terrain2 Texture – Terrain texture gives options to create the look of the landscape.

Weave2 Texture – Weave texture produces a simple basket weave or textile pattern in the relief.


Page 50 Toolbars and Command Icons

Other Command Icons

This section identifies icons from many of the tools in EnRoute. The main intent here is to provide a listing of EnRoute icons in one place for your review. All of these functions are explained in more detail, within the context of the EnRoute functions to which they belong.

Noise Distort - This method allows users to create noise distortion co contours  and reliefs by defining a small number of parameters. It is the simpler of the two
methods.

Noise Distort - This method provides the ability to define a two-pass directional  distortion. It has mare parameters than Method 1, but also gives the user more

control over how the distortion is applied.

Add relief – This option is used to create a raised relief.


Arc by center and two points – Use this command to define an arc by defining its center and two endpoints. It is defined interactively; you can either leave it as an open contour with just the arc, or define it as a closed contour by placing the cursor either outside or inside the arc as it is constructed.


Arc by point and angle – Define an arc by entering coordinates for the center and start, and then defining the angle turned by the arc.


Arc by three points – This is a handy interactive tool to define an arc by clicking  on the start point, then clicking on the end point, and then dragging to define an

intermediate point on the curve.

Arc copy – In the Multicopy function, select this parameter to copy around an arc.



Array copy – Creates multiple copies of an object according to the selected parameters.

Bevel Relief – This tool is chosen to create a beveled relief.

Bevel Relief Edit Tool – This tool allows editing of a relief using a beveled shaped tool.

Blending Relief Edit Tool – This tool will blend the surface of the relief within the parameters specified in the toolbar dialog.



Block Nester - The Block Nester is designed to be used with squares and rectangles. It can be the most efficient and fastest method of nesting. It allows for the option to create a common-line contour. This option is useful for cutting rectangular parts because it prevents “double cutting” of the parts.

Box – Box shaped mesh found in create primitive objects.

Circle by Center and Point – This tool allows you to enter the coordinates for both the center and a point on the circle to define the circle.



Toolbars and Command Icons Page 51

Circle by Center and Radius – Use this tool to click on a circle center and then drag to define its size. Define the circle by coordinates and dimension also.

Circle by corners – Click and drag to define the corners of a boundary box around a circle, or define these corners by precision input.


Circle by three points – This is an interactive tool used to define a circle. Click on the first point then click, hold and drag to define the circle.

Concave polygon – Choose this tool to draw a concave polygon, or star shape.

Cone – Cone shaped mesh found in create primitive objects.

Convex Polygon – Choose this tool to draw a convex polygon.

Corner chamfer – This tool will chamfer the corners of a rectangle. Specific parameters can be entered to determine the radius and placement of the rectangle.

Corner fillet – This tool allows you to place a fillet on the corner of a rectangle to your desired parameters.

Corner reverse fillet – This tool puts a reverse fillet on the corners of a rectangle.

Corner square – When this option is chosen, the corners of the rectangle is square.

Cylinder – Cylinder shaped mesh found in create primitive objects.

Dimension Arrow Height - This parameter determines the height of the arrow.

Dimension Arrow Width– This parameter determines the width of the arrow.




Dimension Decimal position for arc– This parameter sets the number of decimal positions to be displayed for the arc dimensions.

Dimension Decimal position for Line– This parameter sets the number of decimal positions to be displayed for the line dimensions.


Dimension Extension line parameter- This parameter sets the distance that the extension lines start to draw from the start and end points of the dimension.


Dimension parameter Height-This parameter sets the height of the text in the dimensions tool.



Dimension Text Position above- This sets the position of the text above the arrow line.

Dimension Text Position Center- This sets the position of the text in the center of the arrow line.


Page 52 Toolbars and Command Icons

Dimension Text Position Below- This sets the position of the text under the arrow line.

Disc – Disc shaped mesh found in create primitive objects.


Distort Toolpaths – This allows users to modify Island and Hatch fill toolpaths in order to introduce variations that can allow designs to appear hand carved. It is

now possible to add a unique touch to any 3D surface just by adding some variation
to the toolpaths after they have been created.

Dome Relief Edit Tool – This tool is used to edit a relief in a dome shape.

Edit Bridges – The edit bridges tool allows you to edit individual bridges, moving them and changing their parameters.



Edit entry exit – Each cut in a toolpath has its own entry and exit points. Use this tool to edit the points or type of entry and exit.

Ellipse by dimensions – Enter the coordinates for the center of an ellipse and then define its height and width along its two axes.


Ellipse from corner to corner – This tool is similar to the circle command of this  same type. Just interactively click and drag on the corners of a boundary rectangle
to define an ellipse.

Explode selected contours – This tool will separate a selected contour into individual segments.


Faceted mesh to relief – After a mesh is created, it is then added to a relief. If the  faceted option is selected, then the object is applied to the relief surface using its

facets directly.

Flat relief – This tool is chosen to create a flat relief.

Flat Relief Edit Tool – This tool is used to edit a relief using a flat shape.



Horizontal Distance Multicopy – This tool defines the distance horizontally between the objects when using the Multicopy function.

Horizontal Distance Multicopy - This tool defines the distance horizontally

 between objects in Multicopy from the front end of an object to the front end of the next object.


Measure Tool Angle – This tool will calculate the degree of the angle between two selected points on a contour, or three selected points not on a contour.


Measure Tool Area – This tool will calculate the area of a closed contour. If you select more than one contour, it will also add the total area of the selected objects.


Measure Tool Segment - This tool will measure the distance between two points. It will continue to add each selected segment to the total.


Toolbars and Command Icons Page 53

Merge highest relief – This option is used to modify a relief. The new portion of the relief only modifies the existing relief where it is higher than the existing relief.

Merge lowest relief – This option is similar to the Merge Highest option, except that a relief is only modified where the new relief is lower than the existing relief.


Merge selection – The Merge Selection tool is used to join open contours together based on a definable tolerance.


Mesh – Mesh objects are made up of triangles of varying sizes that define their surface.


Mirror Horizontal – This tool reverses the selected contour so that it becomes its mirror image horizontally.


Mirror Vertical – This tool reverses the selected contour so that it becomes its mirror image vertically.


Move Absolute - Absolute move will move the selected object from one point to another precisely or interactively.


Move Corner- The Corner move tool allows you to move the selection based on the points of the bounding box for the selection.



Move Relative- The Relative move allows the user to move the selection by a specific amount in each direction.

Move Text - Select this tool to move the location of the selected text up or down. A


positive value will move up; a negative value will move down.

Multiple Fillet – This tool is used to fillet multiple corners of a selected object.



Path copy – In the Multicopy function this will allow you to create multiple copies along a path specified.

Plane – Plane shaped mesh found in Create Primitive Objects.

Project toolpaths to plane – Use this tool to change the height or angle of existing toolpaths.

Rectangle by dimensions – Enter the parameters to define a corner of a rectangle and then specify its size by height and width.


Rectangle corner to corner - Use this tool to define a rectangle by clicking on one  corner and dragging to define to the opposite corner. Hold the shift key down to
keep the rectangle a square.

Replace relief – This option is also used primarily to modify an existing relief. The  applied profile takes the place of the existing relief wherever the new profile
overlaps the existing profile.

Reset Parameters – This tool is used to reset the ordering parameters of the toolpaths using the Preferences.


Page 54 Toolbars and Command Icons



Reverse Open Contours – This tool will reverse the direction of the selected open contour.

Rounded relief – This tool is chosen to create a rounded relief.

Save Parameters – This tool will save the current parameters to the preferences.

Scale 3 Dimensions – In the scale tool, this option will scale the selection in all 3 axes, based on the scale factors that are defined either precisely or interactively.


Scale 2 Dimensions – In the scale tool, this option allows three-dimensional  objects such as reliefs and meshes to be scaled in just two dimensions. For
example, you can scale a relief in XY dimensions without changing its thickness.

Scale 1 Dimension – In the scale tool, this option allows you to scale a selection in  just 1 direction. Stretch the x-dimension without changing the y or z size of a
selection.

Set start point – Use this option in the edit points tool to set the start point of a contour.



Shape Nester – This option, within the nesting tool provides access to three different nesting algorithms for true-shape nesting of contours, reliefs and toolpaths.

Simulate done – Close the simulation.

Simulate Draw Next Segment – The start of the simulation.

Simulate next tool lift – This will play the simulation until the tool is lifted.

Simulate pause – This will stop the simulation.

Simulate to end of job – This will play the simulation to the end of the job.

Simulate to tool change –This will play the simulation until the tool is finished.




Simulate rewind – In the simulation tool, this is the function to rewind the simulation to play it again.

Single Fillet – This tool is used to interactively place a fillet into a select area of a contour.

Slant Text - Select this option to change the slant of the characters. A positive

 value will cause the letter to lean towards the right, while a negative value will make the letter lean back or to the left.


Smooth mesh to relief – This option implements a means of smoothing out the  facets of the mesh to provide a smoother finished surface when applying the mesh
to the relief.

Toolbars and Command Icons Page 55

Smooth Relief Edit Tool – This tool has a smooth shape to use when editing the existing relief.

Sphere – Sphere shaped mesh found in create primitive objects.


Subtract relief – This option is used to create a recessed relief.

Text Height- Select this tool to change the height of the text objects.

Text position on contour - Select this tool to determine which side of a line or curve the selected text is to be placed.

Text Spacing - Select this tool to change the spacing between the text objects. A

 positive value will increase the spacing; a negative value will decrease the spacing between characters.

Text Width- Select this tool to change the width of the selected text objects.


Texture Relief Edit Tool – This tool allows the user to edit a relief with a texture tool.

Torus - Torus shaped mesh found in create primitive objects.

Vertical distance Multicopy – This tool defines the distance vertically between objects when using the Multicopy tool.


Vertical distance Multicopy – This tool defines the distance vertically between the  objects in Multicopy from the front end of an object to the front end of the next
object.

Page 56 Toolbars and Command Icons

4. Working with Drawings

Creating New Drawings

Menu: File / New

Toolbar: File / New

Click New The keyboard shortcut is Ctrl+ N.
EnRoute supports the Multi Document Interface (MDI), which allows you to have more than one drawing open at a time.
 If you have the Prompt for Plate option turned ON (see “Setting Preferences”), you will be asked
to define the Plate each time you start a new design.

Defining a Plate

Menu: Machining / Define Plate

Toolbar: Libraries / Redefine the current plate


When a new drawing is created, the Define Plate dialog opens.
The Define Plate dialog allows you to specify the dimensions of the material on which you are working, as well as the type of material.

Working with Drawings Page 57

The following options are available:

User

Defined

If this option is selected, you can enter the Origin, Width and Height of the material to be used.

Fit Plate to

Design

If this option is selected, a plate will automatically be created with height and width values based on the current design.

Fit Plate to

Selection

If this option is selected, a plate will be created based on the currently selected contours.

Width

The measurement of the plate along the X-axis.

Height

The measurement of the plate along the Y-axis.

Thickness

The measurement of the plate along the Z-axis.

X/Y Origin

The X/Y Origin is the position of the lower left corner of the plate.

X/Y Margin

If a margin is entered, a second, dashed rectangle is created on the inside of the plate’s edges. The margin is used to help create the layout. It can be very helpful for masking out the locations of clamps.

Surface

Option

Surface at top of plate tells the program that you have set the surface at the top of the material. If you choose surface at bottom of plate, this means that you will set the surface at the top of the table (or bottom of the material).

Wrap Plate

EnRoute supports creating output that will be sent to a rotary axis CNC machine. The Wrap Plate option allows you to automatically set the size of the plate in the X or Y direction so that it is compatible with the design being “wrapped” around

either the X or Y axis when it is output. The correct height or width of the plate is based on the circumference of the wrapped design, as controlled by the thickness

of the plate, which corresponds to the radius of the wrapped cylinder.

For example, if you wrap around the X axis, then the height of the plate will automatically be set to correspond to the circumference of the wrapped cylinder. If the plate thickness is 50mm, then the circumference of 314.1593mm is automatically calculated for the height of the plate.

When you exit the Plate dialog, if Wrap Plate is checked, it will be displayed as wrapped in the drawing. As you work through the design process, you will likely want to primarily view the plate in the unwrapped state. It is easy to toggle between wrapped and unwrapped views using Ctrl-Shift-X to toggle the X axis and Ctrl-Shift-Y to toggle the Y axis.

Material

Clicking on the Material list box will display the types of materials (wood, metal, etc.) that are defined. Selecting the Material Library button will allow you to create a new material type, and the routing speeds associated with that material.

OK

Click OK to accept.

Cancel

Click Cancel to close this dialog.

Save As

Click Save As to save the current parameters as a template. The parameters can then be reloaded from the library by selecting the template from the Template list.

Page 58 Working with Drawings

Remove

Click to remove the plate that is currently defined. You will be returned to the layout window and the plate will be removed.

Material

Library

The Material Library may be accessed from this dialog. This allows you to define new material, change information on previously defined material, and save new or edited information set for specific materials. See “Editing the Material Library” for details.

Creating a Basic Plate

1. Click the Define Plate icon. 
2. Enter the Width (distance along the X axis).
3. Enter the Height (distance along the Y axis).
4. Enter the Thickness of the material.
5. Enter values for Margin and Origin if desired.
6. Choose a Material Type. (This is optional).
7. Check to surface at the top or bottom of plate.
8. Click OK to create the plate.

Create Plate from Selected Contour 

The user has the choice to create a plate that is not a rectangle. This allows users to define different material sizes in one drawing. Any shape of plate can be defined simply by drawing a contour, selecting that contour and clicking on the icon.
This feature can be used with the nesting feature when a remnant has been created. By selecting that contour and clicking on the Create plate from selected contour icon, the shape of that remnant will be the next plate. This allows the user to easily utilize the leftover material for another part of the job.
Example:
This shows nesting the objects and creating a remnant from the remaining material. Select the remnant contour and click on the Create plate from selected contour icon. This will create the plate that represents the remaining material.
Any contour shape can be used with this feature.

Working with Drawings Page 59

Plate Panels

With this tool the user can define a specific area of the plate to create the output for the toolpaths. This is very useful for oversized projects that may not fit all at once on the table. By defining separate areas to output the toolpath information, the project can be cut in separate phases. This would allow the material to be very carefully repositioned in order to cut material that may be to long for the machine to cut in one application.
1. Click the Define Plate icon. Follow the directions above for creating a Basic Plate. You will want the plate size to reflect the size of the material that you wish to cut.
2. Click on the Define plate panels for oversized designs icon.  This will place a green border within the plate.


3. Click outside of the border and drag to the location that you wish to create your panel.
4. You can then use the F2 button to open a dialog so that you can specifically locate the position of the border. Click on the bright green line and then enter the location parameter. The pink line shows the location of the border of the panel. Click OK.

Page 60 Working with Drawings



5. The shaded area is the active area to output the toolpaths. Toolpaths that cross the boundary of the plate panel will be cut off when they are output.

6. To change the active panel, simply click on the Define plate panels for oversized designs icon . Click in the area of a different panel. Either press Return, or click the F2 button to open the dialog and click OK. The shaded area is now in the selected area for the output of the toolpaths
.

Working with Drawings Page 61

Using Plate Templates

Templates are used to store frequently used settings. Selecting the template reloads the information saved in the template.

Saving a Template

1. Enter the desired information in the Define Plate dialog box.
2. Click Save As.
3. Enter the name of this template and click OK.
4. This template will now be added to your plate template library.

Using a Template

1. Click on the Template list and the saved plate templates will be displayed.
2. Select the desired template.

Opening a Drawing

Menu: File / Open

1. Click Open or Ctrl +O.
2. Select the folder and the file that will be opened. When you have selected a file to be opened, if it was saved in EnRoute 5 or above, it will show a preview of the file in the panel on the right side of the dialog.
3. Press Enter or click Open.

Page 62 Working with Drawings

Saving a Drawing

Menu: File / Save

1. From the File menu, select Save or Save as
2. If you have selected the Save as command or you are saving the document for the first time, the Save dialog is displayed. Enter the name and the location that will be used to save the document.
3. Click Save.

 The file will be saved in the folder as specified. Be sure that you know where the file is being saved so that you will be able to locate it the next time you want to open it.

Closing a Drawing

Menu: File / Close

1. From the File menu, select Close.
2. If your file has changed since the last time it was saved, a dialog is displayed asking if you want to save the current file.
 Click Yes to save the file before closing it.
 Click No to close the file without saving the changes.
 Click Cancel to keep the file open.

Importing a Design

Menu: File / Import.

1. Click Import. 
2. Select the file format, folder and the file that will be imported.
3. Press Enter or click Open.

 See the Preference command located in the Setup menu for options regarding the Import command.

 Bitmap graphics must be converted into contours before they can be

used to generate toolpaths. See “Vectorizing Bitmaps” for details.

Working with Drawings Page 63

Exporting Design Information

Menu: File / Export

EnRoute can export a design to a number of different drawing formats.

 Generally, only contours will be exported. When exporting to DXF, it is possible to also choose to export toolpaths, but it’s not recommended unless you have a specific use for the toolpaths in this form. It is also possible to export meshes to formats that are compatible with mesh objects, such as DXF and STL. The only way to export a Relief is to first create a mesh object using the relief.

1. Click Export
2. Select the file format, folder and the file name.
3. Type the name of the file to be exported in the File Name box.
4. Select the directory and drive you want the file exported to.
5. Press Enter or click Save.

Printing

Menu: File / Print

Use the Print command to print the active design.
1. Click Print This will open the Print dialog.
2. Select the type of print option.

Design

Select this option to send all the contours that exist in the current layout to the printer.

Selection

Select this option to send only the selected contours to the printer.

Window

Select this option to send the layout window to the printer. Exactly what is displayed on screen is what is sent to the printer.

Plate

Select this option to pint only the plate.

3. Click OK.

Setup

Click the setup button to open the print setup dialog.

Page 64 Working with Drawings

Calculator

Menu: File / Calculator

If you find the need for a calculator, EnRoute provides quick access to the Windows calculator with a simple click on the calculator icon. 

Snapshot

Menu: File / Snapshot

EnRoute has the ability to take a snapshot of the active view.
1. Click on the Snapshot icon. 
2. Select the file type and location that you wish to save the file.
3. Click the Save button. The snapshot will be saved as a bitmap in the jpg format.

Measure

Menu: File / Measure 

The Measure tool provides a handy way to calculate lengths and distances, angles between contour segments, and areas of closed contours.

Segment Length - This tool will measure the distance between two points. It will continue to add each selected segment to the total.

Working with Drawings Page 65

Angle Measure Tool - This tool will calculate the degree of the angle between two selected points on a contour, or three selected points not on a contour.

Area Measure Tool - This tool will calculate the area of a closed contour. If you select more than one contour, it will also add the total area of the selected objects.


1. Click on the Measure tool to activate the Precision Toolbar.
2. Select the icon for measurement type: Segment, Angle or Area.
3. Using the snap tools will help you to easily select specific points in order to get accurate measurements.
4. The Precision Toolbar displays the information for the function that you are performing. In addition, temporary dimensions are displayed showing the measurement.
5. Right click in order to reset the measurement value. If you click for measurements without resetting, the new measurements will continue to be displayed. Right click any time to reset and clear the displayed measurements.
6. Changing from a length measurement to an angle measurement also resets the display.

Page 66 Working with Drawings

5. Creating Contours


A selection of drawing tools is provided to allow you to create your design elements. Design elements may be created interactively by clicking and dragging, or they may be created precisely by entering desired values in the Precision Toolbars.

Line, Polyarc Bezier Curve or Draw a Curved Contour

Drawing a Line

Menu: Draw / Draw Line

Toolbar: Construction / Draw Polyarc / Draw Line

The Line tool draws a straight line segment connecting two points.
1. Click and hold Polyarc  then select Draw line. 
2. Click at the desired starting point then move the cursor to where you want the line to end and then click again.
 Hold the SHIFT key down while drawing to force the tool to create only horizontal and vertical lines.
You can also press the F2 key to enter each starting and ending point’s coordinates into the Precision
Input Center. Enter each point’s coordinates into the Xand fields and click OK.

Polyarc

Menu: Draw / Draw Line

Toolbar: Construction / Draw Polyarc / Draw Polyarc

The Polyarc tool allows you to construct a series of lines and arcs to form a new contour. Although it is always possible to construct lines and arcs as separate entities and then join them together to form a contour, this tool allows you to accomplish both tasks together.
After activating the Polyarc command, the Precision Toolbar is activated, allowing you to choose between line and arc mode. The following table defines the buttons in the Precision Toolbar that present the available options for constructing lines and arcs.
 Line - This toggles the segment creation mode to the line mode.  Arc - This toggles the segment creation mode to the arc mode.

Creating Contours Page 67


Position - This allows you to define a position for either the start of a segment or the end of the active segment.

Direction – This allows you to define a direction for either the line or arc you are creating. If you are defining a line, the direction is the direction of the line. If you are defining an arc, the direction is the direction of the tangent to the arc relative to the previous segment. If it is the first segment, then the direction is relative to a line to the right.

Arc Center – This is only available in arc mode and is the center of the arc you are creating.

 Radius – This is the length of the radius of the arc you are creating.


Sweep Angle – This is the sweep angle of the arc you are creating.
As you use the tool, you see that only the options that are possible based on where you are in the command are available at any given time. If you are in line mode, then the arc parameters are disabled.
The idea with this tool is to construct segments, one at a time, and to use the method that fits the information you have available. Construction of the segments can be done either interactively or by entering values into the available edit boxes in the Precision Toolbar. This tool was designed to be used exclusively in the top view because you are creating arcs, and EnRoute expects arcs to be planar in the x-y plane.

Constructing a Line Segment – following are the simple steps required to create a line segment.

 Activate the Line Mode.


If this segment is the first segment in you Polyarc contour, then either snap/click to the correct location in the drawing or define the correct x- and y-coordinates in the toolbar in order to start the segment.

 Then define the next position for the endpoint of the line.


The other option for the endpoint of the line is to switch to the direction mode and then define an angle and distance in order to complete the line segment.

 You are now ready for the next segment.

Constructing an Arc Segment – following are the steps required to create an arc segment. With an arc segment, EnRoute is trying to get enough information to define the arc. As soon as enough information has been defined then the arc is created. You can use many different combinations of information – start point, direction, radius, center point, sweep angle, and end point – to define the arc. The key is to remember that you are always trying to define enough parameters to allow the arc to be finalized.

Page 68 Creating Contours

The following examples demonstrate how arcs can be constructed in different ways.

Example 1

 Activate the Arc Mode.


If this segment is the first segment in you Polyarc contour, then either snap/click to the correct location in the drawing or define the correct x- and y-coordinates in the toolbar in order to start the segment.

Then define the next position for the endpoint of the arc. The endpoint allows the arc to be constructed because the arc is assumed to be tangent to the previous segment. If it’s the first segment, then the tangent is assumed to be 0 degrees. With the endpoint and the tangent known, the rest of the arc parameters can be calculated and the arc constructed.

 You are now ready for the next segment.

Example 2

 Activate the Arc Mode if necessary.


If this segment is the first segment in you Polyarc contour, then either snap/click to the correct location in the drawing or define the correct x- and y-coordinates in the toolbar in order to start the segment.

Now switch to direction. You can now either define the direction by clicking on a point or by defining the direction in the edit box.

The position mode is activated, so just click on a point or define its coordinates in order to complete the arc.

 You are now ready for the next segment.


Example 3

Activate the Arc Mode if necessary.

If this segment is the first segment in you Polyarc contour, then either snap/click to  the correct location in the drawing or define the correct x- and y-coordinates in the

toolbar in order to start the segment.

Now switch to center point. You can now either define the center of the arc either by clicking on a point or by defining the point in the edit boxes.

Or

Now you just need to define either the endpoint of the arc or the sweep angle in order to complete this segment. Choose the preferred mode and then either enter the information in the toolbar or click on the appropriate point in the drawing. This will complete the segment.

Creating Contours Page 69



You are now ready for the next segment.
If you try these examples in your drawing, it demonstrates how arcs can be constructed very precisely by providing just enough information to construct each segment. When you are constructing precise parts that are based either on customer specifications, or on a drawing that you have been provided, this tool allows you to work your way around the part using the information available for each segment.

Bezier Curve

Menu: Draw / Draw Line

Toolbar: Construction / Draw Polyarc / Draw Bezier Curve

Bezier curves provide a way of drawing curved lines on a computer. Each section of a Bezier curve is defined by four points: its beginning and end points, and two handle points which determine the shape of the curve.

Handle Point

End Point

End Point

Handle Point

A contour created using the Bezier tool will typically be drawn with multiple segments. Each segment can either be drawn as a Bezier segment or as a straight line segment.

1. Click and hold  then click Draw Bezier curve
2. To place the first point in the curve, do one of the following:
3. Click once without dragging to place the point. This will make the first segment a straight line.
4. Click to place the starting point and drag to create its handle. This will make the first segment a curve.
5. For all subsequent points in the curve, click to place the point and drag to create its handle. If you do not drag to create a handle, the next line segment will be a straight line.

Page 70 Creating Contours

6. Right-click to release the tool and end the curve.

 If one of your segments does not come out exactly right, keep going and finish the curve: you can easily come back and edit the segments later. See “Editing Points on a Curve or Contour” for details.

You cannot create a Bezier curve using the Precision Input Center. You must create the curves with the mouse or other pointing device.
Example:
To draw a simple s-curve:


1. Click and hold then click Draw Bezier curve

2. Click to create the upper right-hand starting point of the curve.
3. Click one grid unit to the left of the first point and drag one additional point to the left. This sets you up for the creation of the first curve.

4. Click one grid unit below the second point and drag one unit to the right.

Creating Contours Page 71

5. Click one grid unit below the third point and drag one unit to the left. 

6. Click one grid unit to the left of the fourth point and right-click to finish drawing the curve.

Sketch

Menu: Draw / Sketch a curved contour

Toolbar: Construction / Draw Polyarc /Sketch a curved contour

This tool allows freehand drawing of contours.


1. Click and hold then click on Sketch a curved contour.
2. Left click and hold while moving the mouse to create the contour. As soon as you release the left mouse button, the contour will be constructed. EnRoute has captured all of the mouse movements, and it then constructs a smoothed contour that represents what you drew. If you move the mouse back around so that it is close to where you started the contour, EnRoute will close the contour when it is finalized. The contour is constructed using a combination of lines and arcs.
3. Right click to exit the tool.

Rectangle

The rectangle tool was designed to allow the user to construct rectangles using whatever method is most convenient. All of these construction methods are available within one tool, and you can switch between them at any time. Also, you can define rectangles either interactively or precisely, and you can combine both methods. Following are some specific instructions for creating rectangles.

Drawing a Rectangle by Corners

Menu: Draw / Rectangle

Toolbar: Construction / Rectangle / Corner to Corner

Page 72 Creating Contours

1. Click the Rectangle Icon. This will open the Precision Toolbar. Select the Draw from

Corner to Corner. 

2. Click to place the first corner, and then drag the mouse to the location of the opposite corner and click the mouse again to place the rectangle.
3. If desired, you can continue to create more rectangles. Repeat step 2 to place the rectangles.
4. Right-click to end the rectangle function.
 Hold down the SHIFT key to force the software to draw only squares.
You can also enter each corner’s coordinates into the and fields and click Apply.
 The Corner icons in the Precision Toolbar allow you to create a rectangle with radiused corners.
Select the style of corner you want and the size of the radius.

Rectangle by Dimensions

Menu: Draw / Rectangle

Toolbar: Construction / Rectangle / By Dimensions

To draw a rectangle by defining a starting point and the height and width of the rectangle:
1. Click the Rectangle Icon. This will bring up the Precision Toolbar. Select Draw by

Dimensions

2. In the Precision Toolbar, click the reference grid button that corresponds to the corner, side or center point that will be used to position the rectangle.
3. Enter the Height and Width values to define the size of the rectangle.
4. Left click to place the rectangle or enter the X, and Y coordinates for the positioning point.
5. To create a rectangle with radiused corners, select the style of corner you want and the size of the radius.

 The selected corner option will only be constructed if both the height and width of the rectangle are large enough to allow the size (radius) of the corner.

6. Click Apply. The rectangle will be placed in the workspace.
7. If desired, you can continue to draw more rectangles. Left click to place additional rectangles with the same values or enter the new values for the rectangles in the fields as before and click Apply to draw.
8. Right-click to end the rectangle function.

Creating Contours Page 73

Circle

Like the rectangle tool, the circle tool provides several options for defining a circle. All of the options are available in one tool, and you can define coordinates either interactively or precisely.

Drawing a Circle by Center and Radius:

Menu: Draw / Circle

Toolbar: Construction / Circle / By Center and Radius

1. Click the Circle Icon. From the Precision Toolbar select By Center and Radius
2. Enter the value for the Radius of the circle. Left click the mouse to place the circle.
3. If desired, you can continue to create more circles of the same size by left clicking the mouse to place the additional circles. The circles can also be precisely placed by entering the x and y coordinates for the center of the circle and click Apply.
4. Right-click to end the circle function.

 After defining the radius for a circle, you can place multiple circles with that radius just by clicking to define center locations.

Drawing a Circle by Center and Point

Menu: Draw / Circle

Toolbar: Construction / Circle / By Center and Point

1. Click the Circle Icon. This will bring up the Precision Toolbar. Select Circle by Center and point
2. Click to place the center point of the circle, then drag to define the point on its radius. Click the mouse again to complete the circle.
3. If desired, you can continue to create more circles. Repeat step 2.
4. Right-click to end the circle function.
5. You can also enter the data for the center and the point into the corresponding fields. Click

Apply.

 Don’t forget that you can use snaps to precisely locate the points on your circle.

Drawing a Circle by Three Points

Menu: Draw / Circle

Toolbar: Construction / Circle / By Three Points

1. Click the Circle Icon. This will open the Precision Toolbar. Select By Three Points.

Page 74 Creating Contours

2. Click to place the first point on the circle.
3. Click to place the center point on the circle, then drag to define the third point. Click the mouse again to complete the circle.
4. If desired, you can continue to create more circles. Repeat steps 2 and 3.
5. Right-click to end the circle function.
You can also enter the data for the points into the corresponding and fields. Click Apply.

Drawing a Circle by Corners

Menu: Draw / Circle

Toolbar: Construction / Circle / Circle by Corners

1. Click the Circle Icon. This will open the Precision Toolbar. Select Circle by Corners
2. Click to place the first corner, then drag to define the opposite corner. Click the mouse again to complete the circle.
3. If desired, you can continue to create more circles. Repeat step 2.
4. Right-click to end the circle function.
You can also enter the and coordinates for the corners and click Apply.

Arc

The arc tool provides three different methods for constructing an arc. All of the methods allow both interactive and precise definition of points and parameters. After the arc is constructed, it is a separate open contour. If your design is comprised of several open contours before certain types of toolpaths, such as fills, may be applied.

Drawing an Arc by Center, Start and Finish

Menu: Draw / Arc

Toolbar: Construction / Arc / By Center, Start and Finish

1. Click the Arc Icon. This will open the Precision Toolbar. Select Arc by Center, Start and
Finish. 
2. Click to define the arc center.
3. Click to define the start point.
4. Click to define the arc endpoint.
5. If desired, you can continue to create more arcs using the same method.
6. Right-click to end the arc function.
You can also enter the data into the and fields for each point and click Apply.

Creating Contours Page 75

Drawing an Arc by Center, Radius and Angle

Menu: Draw / Arc

Toolbar: Construction / Arc / By Center, Radius and Angle

1. Click the Arc Icon. This will open the Precision Toolbar. Select Arc by Center, Radius and

Angle

2. Enter the X and Y coordinates for the Center point.
3. Enter the Radius parameter.
4. Enter the Start Angle parameter
5. Enter the Sweep angle parameter. Left click to place the arc. Left click to place more arcs with the same parameters.
6. If desired, you can continue to create more arcs using the same method.
7. Right-click to end the arc function.
You can also enter the data into the and fields for the points and enter the degree of the angle and click Apply.

Drawing an Arc by Three Points

Menu: Draw / Arc

Toolbar: Construction / Arc / By Three Points

1. Click the Arc Icon. The Precision Toolbar will open. Select By Three Points
2. Click to define the start point.
3. Click to define the end point.
4. Click or drag to define a third point along the arc.
5. If desired, you can continue to create more arcs using the same method as the first.
6. Right-click to end the arc function.
You can also enter the data in the and fields for the coordinating points. Click Apply.

Ellipse

The ellipse tool works much the same as the other drawing tools, including three options for construction method. A new method in this tool allows the ellipse to be constructed by defining the angle of the major axis of the ellipse and the height and width. This allows the ellipse to be rotated so that the major axis is not the x axis when it is constructed.

Page 76 Creating Contours

Drawing an Ellipse by Height and Width

Menu: Draw / Ellipse

Toolbar: Construction / Ellipse / Draw by Height and Width

To draw an ellipse by defining a center point and the height and width:
1. Click Ellipse Icon. From the Precision Toolbar select Draw by Height and Width
2. Enter the parameter for the center point.
3. Enter the Height and Width values.
4. Enter the Angle parameter for the ellipse.
5. Click Apply. The ellipse will be placed in the workspace.
6. If desired, you can continue to draw more ellipses. Left click to place more ellipses with the same parameters or enter the new values for the ellipses in the fields as before and click Apply to draw.
7. Right-click to end the ellipse function.

Drawing and Ellipse by Major and Minor Axis

Menu: Draw / Ellipse

Toolbar: Construction / Ellipse / Major and Minor Axis

1. Click the Ellipse Icon. This will open the Precision Toolbar. Select Ellipse by Major and

Minor Axis. 

2. Left click to place the center point, drag and click to define the angle of the major axis and the width of the ellipse, drag and click to define the height of the ellipse.
3. You can now change to the Ellipse by Height and Width  method to continue placing ellipses with the same parameters. The preview will show on the screen, simply left click to place another ellipse.

Drawing an Ellipse by Corners

Menu: Draw / Ellipse

Toolbar: Construction / Ellipse / Corner to Corner

To draw an ellipse by identifying opposite corners of a bounding rectangle:

Creating Contours Page 77

1. Click the Ellipse Icon. This will open the Precision Toolbar. Select Draw from Corner to

Corner. 

2. Click to place the first corner, then drag to define the opposite corner. Click the mouse again to complete the ellipse.
3. If desired, you can continue to create more ellipses. Repeat step 2.
4. Right-click to end the ellipse function.
You can also enter the data into the and fields. Click Apply.

Component Creator

The Component Creator is a fun new tool in EnRoute that provides a way to create slotted parts that assemble to create something as simple as a rectangular shelf, all the way up to a complex assembly using EnRoute’s surface creation capabilities. Just select your base object, either a contour or a relief, get in the tool, define a few parameters, and then let EnRoute create all the ready-to-cut parts.

Menu: Draw / Create Shelf Components

Toolbar: Construction / Create Shelf Components

Position

Position the grid within the container. You will see the coordinates change as you click and drag the grid interactively. You can also enter coordinates precisely to put the grid right where you want it.

Size

The X and Y dimensions of the grid. The Z value defines the depth of the components if you have the Return option checked.

Angle

The rotation angle of the component grid. This can be used to add a creative flair, or to add function to your bookshelf so all the books will stay standing.

Shoulder

This value relates to the parts if they are created using the Dish and Return options. If so, then this specifies the width of a “shoulder” that provides the specified Return depth on the parts.

Page 78 Creating Contours

Cross Hatch

Check if you want to create both horizontal and vertical components. If you want to create only horizontal components, then uncheck this option.

Loft

Check if the component is based on a relief and you want the front of the parts to follow the relief.

Return

If checked, the parts will be constructed with the depth as specified by the Z

value in the Size parameter.

Notch

Check to create a notch in the components so they fit together as a grid.

Dish

Check if the component is based on a relief and the back of the components will follow the shape of the top of the relief.

Layout

Check to create the 2D contours of each part so that it can be toolpathed and cut.

Label

Check if you wish to label the parts.

Model

Check to have EnRoute create a 3D model of the assembly so that it can be reviewed to make sure the parts will fit together as you intended.

Material

Thickness

The thickness of the material you plan to use. This controls the width of the notches.

Glue Gap

The amount of the gap you wish to allow for glue when assembling the parts. This is also a way to control how tightly the parts fit together.

Notch Gap

The amount of the gap needed to allow the tool to cut so that tool dimension does not interfere with the assembled joint. A good value to use here is the radius of the tool you plan to use to cut the parts.

1. First, draw a contour that represents the shape of the assembly. You can also create a relief that represents the front surface assembly.
2. Select this shape and click on the Component Creator icon within the Construction

Toolbar.


3. In the toolbar, enter the information required. The parameters are defined in the previous table. You have many options available to create a one-of-a-kind artistic piece or something as simple as dividers for a drawer or shelf. As you define the parameters, the graphic is updated to reflect the choices.
4. Press the Apply button to create the component parts.

Creating Contours Page 79


5. The parts of the components are created to the right of the geometry and if you have checked the Model parameter, switch to the perspective view to see a rendering of the assembled shapes you are creating.

6. The last step is to move the component parts to the plate and apply toolpaths for cutting.
7. This example shows that you can create components that follow the shape of a relief.

Page 80 Creating Contours

Polygon

Menu: Draw / Polygon

Toolbar: Construction / Polygon / Convex or Concave

The polygon tool allows you to create multi-sided, closed contours such as pentagons and stars.
1. Click the Polygon Icon. This will open the Precision Toolbar
2. In the Precision Toolbar, select the type of contour you want to create: either a convex
polygon  or a concave polygon. 
3. Set the number of Points for your convex shape or concave shape.
4. When drawing a convex polygon, simply left click to represent the center of the polygon, drag the mouse to the outside point and then click to end. At this point, you can now enter the coordinates for the center point and one outside point as well as the number of corners for
the polygon. Any changes that you make to the coordinates are shown as a preview. Once you click apply the polygon is placed in the workspace.

Creating Contours Page 81

External Radius

Internal Radius


5. If you are creating a concave polygon, set the Internal Radius for the circle that the inner vertices intersect.
6. Click Apply to draw the polygon.
7. If desired, you can continue to draw more polygons. Enter the new values for the polygons in the fields as before and click Apply to draw.
8. Right-click to end the polygon function or press Close.

Text

Menu: Draw / Text

Toolbar: Construction / Text

The Text tool allows the user to place text and then edit it to change parameters such as size, font style and spacing. You are also able to place text on a curve or an arc.

EnRoute includes the ability to place and edit single-stoke fonts. Rather than the more typical outline fonts, single-stroke fonts utilize a single contour to define the letter. This type of lettering is typically used for marking purposes utilizing an engrave toolpath strategy.

Text Precision Toolbar

Shown below is the first section of the toolbar.


Font Style Preview of the selected font

This is the right section of the Precision Toolbar.

Page 82 Creating Contours


Select this option to change the height of the created text objects. The height of  the character is a nominal height based on the font definition, and should not be
considered to be the actual height of a particular letter.
Select this option to change the slant of the characters. A positive value will  cause the letter to lean towards the right, while a negative value will make the
letter lean back or to the left.

Select this tool to change the width of the selected text objects. It is a factor to adjust the widths relative to the base width.
Select this tool to change the spacing between the text objects. A positive  value will increase the spacing; a negative value will decrease the spacing
between characters.

Select this tool to move the location of the selected text up or down. A positive value will move up; a negative value will move down.

Click on the preferred alignment of the text. Align Left, Align Center, or Align
Right.

Select this tool to determine which side of a line or curve the selected text is to be placed.

1. Click the Add Text Icon. This will open the Precision Toolbar.
2. Click to place the cursor in the workspace. To place the text on an arc or curve, simply click on the contour at the point you wish to start your text. The icon may show slanted to the angle of the arc or curve. Continue with the following steps.
3. Select the text style. A preview of the text is shown the right of the text selection dialog. All
TrueType fonts that are installed on your computer are available to you.
4. You may click the arrows in the height field to adjust the nominal height of the text objects.
The cursor will adjust in size to give you a preview of the size.
5. Type the text.
6. Press Close to exit the Text tool.

Creating Contours Page 83

Editing Text Objects

1. Select the text objects to edit by left clicking and dragging the edit selection box around the objects that you wish to edit. Objects can be selected individually or as a group.
2. Make changes to the text using the tools available to edit the text. A description of the tools is listed in the above section, and they work the same as when the text is first created.

Edit Spacing of Characters

Menu: Draw / Text / Edit Existing Text

Toolbar: Construction / Text / Edit Existing Text

1. Click and hold the Text Icon. This will open the flyout menu. Click on the Edit

Existing Text Objects icon.

2. Click on the text to edit.

Green Point Blue Point Red Point

Green Point

Click and drag the green point to move the starting point for the line of text.

Blue Point

Click and drag the blue points to adjust the spacing

between specific letters.

Red Point

Click and drag the Red point to equally adjust the spacing of the characters for the entire line of text.

Page 84 Creating Contours


This example shows that the Text was moved using the Green start point.

Convert Text Objects to Curves 

Menu: Draw / Text / Convert Text Objects to Curves

Toolbar: Construction / Text / Convert Text Objects to Curves

In order to toolpath the Text Objects, they must first be converted to curves. Any of the toolpath functions will make this change automatically, or you can use this tool to convert text to contours.
1. Select the Text Object(s).

converted they will show with the standard color for contours.


Text Object Converted to Curves

Creating Contours Page 85

Geometry Creation Wizard

Shape Wizards are tools in EnRoute that provide a method for creating objects using parameters rather than drawing them “manually” using EnRoute’s drawing tools. The created contours can range from relatively simple shapes to more complex parts that require several shapes. Parameters can be saved so that getting back to the same parts at a later date is as simple as opening a saved template.

Click and hold the icon to open the flyout menu. Click on the icon of the tool that you would like to work with. This tool will then remain as the Shape Wizard tool in the Construction Toolbar for easy access.


There are currently 14 or 15 wizards available in EnRoute. Since these can easily be added as plug- ins, the list of tools can change as new tools are added. Two of the current tools are described in the following sections – the simple Cone Wizard, and the more complex Boxster.

Cone Wizard

Toolbar: Construction / Cone Wizard

The Cone Wizard allows you to create precise cone shapes. The Template feature allows you to save the different shape parameters so that you can quickly and easily call up the shape and apply it to your design.

Page 86 Creating Contours


1. Enter the parameters of the cone shape that you wish to create.
A preview of the shape will show in pink in the position of the entered coordinates.
Click Apply to accept the shape. The contour will then be shown in black.

2. You are able to save the shapes that you have designed so that you can easily recall the shapes for your design.
Click the Save button.

3. The Template Dialog will open up.
Enter the name of the shape in the dialog and click OK.

Creating Contours Page 87

Boxster

Toolbar: Construction / Boxster

The Boxster Wizard was created in order to provide a simple method for creating cabinet parts in EnRoute using a pre-defined construction method. It uses blind dado joints, allowing the user to define sizes, material thicknesses and other parameters. This tool is not intended to meet the needs of a commercial cabinetmaker, but rather provide a method for creating simple cabinet boxes, likely for use in a workshop or garage. Commercial cabinetmaking will require much more control over cabinet types, materials, and construction methods.

Box Width - Width of the cabinet Box Height - Height of the cabinet Box Depth - Depth of the cabinet

Side Thick - Thickness of material for the side of cabinet

Bottom Thick - Thickness of material for the bottom of cabinet

Top Thick - Thickness of material for the top of cabinet

Back Thick - Thickness of material for the back of cabinet

Edge Band Thick - Thickness of the edge bank material used

Page 88 Creating Contours

Fixed Shelf - The location of the shelf

Shelf Gap - The size of the gap between the shelf and the front of the cabinet. (moveable shelves)

Number of shelves - The number of shelves to be created for this cabinet.

Hole Spacing - The distance between the shelf holder holes vertically

Hole Diameter - Size needed for shelf hardware.

Double Door - 2 doors side by side

Stacked Door - 2 doors 1 over the other

Hinge Left - If checked the hinges will be on the left

Reveal - The measurement that the door is offset from the edge of the frame

Hinge Relief - The distance the first hinge is from the top of the cabinet

Hinge Spacing - The distance between the hinges. EnRoute will then determine the correct number of hinges.

Creating Contours Page 89


Traditional ‘upper’ cabinets will typically contain only doors, while ‘lower’ cabinets might contain drawers rather than doors. This tab lets you define drawers, including number and size of drawers for a lower cabinet design.

Number of Drawers - The number of drawers for this cabinet.

Top Drawer Height - The height of the top drawer.

Middle Drawer Height - The height of the middle drawer.

Bottom Drawer Height - The height of the bottom drawer.

Equal Drawer Height - When this is checked all drawers will have the same height.

Box Material Thickness - The Thickness of the material used for the cabinet.

Bottom Thickness - The distance from the bottom of the cabinet that the pocket will be cut for assembling the cabinet.

Box side Clearance - The distance from the side of the cabinet that the pocket will be cut.

Box End Clearance - Distance from the back of the drawer to the back of the cabinet.

Rabbet Depth - The depth of the pocket cut into the material to assemble the cabinet.

Glue Gap - This measurement allows for the space the glue fills.

End Gap - The internal gap between the end of the male and female portions of the dado joint. Because you are using a round cutting tool, you typically need to accommodate the radius of the tool with this dimension.

End Clearance - The distance from each end of the dado joint to the edge of the part.

Hole Spacing - the distance between holes drilled for the assembly of the cabinet.

Hole Diameter - is determined by the size of the screws that will be used to assemble the cabinet.

Page 90 Creating Contours


This wizard assumes the use of European-style hinges on the doors. These are the most common hinges used on the frameless style of cabinet. Notice that the assumed unit for these parameters is millimeters.

Hinge Cup Diameter - Refers to the size of the hinge.

Hinge Cup Offset - The offset from the edge of the door to the edge of the hinge cup.

Hinge Hole Diameter - The size of the holes that will be drilled for the pilot holes for the screws to fasten the hinges.

Hinge Hole Spacing - Spacing for the location of the hinge hardware.

Hinge Hole Offset -The offset to the centers of the hinge holes from the edge of the door.

Plate Hole Diameter -Size of pilot hole for the hinge plate hardware.

Plate Hole Spacing - Spacing for the hinge plate hardware

Plate Hole Offset - The offset from the edge of the cabinet side to the pilot holes of the hinge plate.


Shape wizards typically create their results within the current EnRoute drawing. The Boxster provides the option of creating each part in its own drawing file in order to facilitate the use of this wizard with EnRoute’s Automatic Toolpath functions

Multiple Drawings - When this is checked, each part will be created either in its own EnRoute drawing of in its own DXF file.

Export As -This provides three options.

No Export means the parts will be created in the active drawing.

EnRoute means the parts will be created in EnRoute Drawings, and DXF will create separate DXF files for the parts.

The DXF option should be selected if you plan to process the parts using the ATP.

Filename Prefix - When multiple drawings are created, each drawing receives a name that is descriptive of the part. The prefix allows you to add to the filename in order to distinguish your projects, and to keep files from being overwritten.

Creating Contours Page 91


This image shows the geometry that is created using the Boxster wizard for one cabinet.

Dimensions

Menu: Draw / Dimension

Toolbar: Construction / Dimension

EnRoute contains a variety of dimension tools that you can use to display the measurements of lines and angles. Using the available snap tools along with the dimension tools makes it easy to establish the dimensions of an object.

Single Dimension – This tool allows you to determine the dimension between two selected points.



Angle Dimension – This tool allows you to determine the angle of two selected contours.

Radius Dimension – This tool allows you to determine the radius of a selected circle.

Diameter Dimension – This tool will determine the diameter of a selected contour.



Leader Dimension – This tool allows you to place a leader arrow in the selected  location of the drawing.

Page 92 Creating Contours

Single Dimension Tool

Menu: Draw / Dimension / Single Dimension

Toolbar: Construction / Dimension / Single Dimension

1. Click on the Single Dimension Icon
2. Select the first point.
3. Select the second point.
4. Drag the mouse to the position you want to place the dimension information.
5. Click to place the dimension.
6. You can then go on to create the next dimension or right click to exit the tool.

Angle Dimension Tool

Menu: Draw / Dimension / Angle Dimension

Toolbar: Construction / Dimension / Angle Dimension

1. Click on the Angle Dimension Icon
2. Select the first contour.
3. Select the second contour.
4. Drag the mouse to the position you want to place the dimension information.
5. Click to place the dimension.
6. You can then go on to create the next dimension or right click to exit the tool.

Radius Dimension Tool

Menu: Draw / Dimension / Radius Dimension

Toolbar: Construction / Dimension / Radius Dimension

1. Click on the Radius Dimension Icon
2. Click on the contour.
3. Drag the mouse to the position you want to place the dimension information.
4. Click to place the dimension.
5. You can then go on to create the next dimension or right click to exit the tool.

Creating Contours Page 93

Diameter Dimension Tool

Menu: Draw / Dimension / Diameter Dimension

Toolbar: Construction / Dimension / Diameter Dimension

1. Click on the Diameter Dimension Icon
2. Click on the contour.
3. Drag the mouse to the position you want to place the dimension information.
4. Click to place the dimension.
5. You can then go on to create the next dimension or right click to exit the tool.

Leader Dimension Tool

Menu: Draw / Dimension / Leader Dimension

Toolbar: Construction / Dimension / Leader Dimension

1. Click on the Leader Dimension Icon
2. Click on the contour.
3. Drag the mouse to the position you want to place the Leader lines.
4. Click to place the line. Using the Text tool you are able to place the text on this line if you choose to.
5. You can then go on to create the next dimension or right click to exit the tool.

Page 94 Creating Contours

6. Contour Editing

Editing Points on a Contour

The Edit Points tool allows you to manipulate lines, curves and points in contours. To edit a contour:
1. From the Draw menu select Edit Points
2. Select the contour.

 Notice that as you place the cursor over a segment, the cursor indicates whether it is a line, arc or curve.

Right-clicking on a segment with the mouse opens a shortcut menu listing commands that are specific to the contour that you are working on.

Pressing F2 will display the Precision Toolbar, which will allow you to precisely place each point.

Edit Points Flyout Menu

The Edit Points tools can also be accessed through the Contour Editing Toolbar. Click and hold the
Point Edit Tool. This will open the Flyout toolbar to access other Point Edit Tools.

Editing a Line Segment

1. From the Draw menu select Edit Points
2. Select the contour.

Contour Editing Page 95

3. Click and drag the contour points to move them.
4. To convert a line into an arc, click and drag on the line segment.
5. To convert a line into a curve, right-click on the line and select Convert to curve.

Editing a Bezier Curve

1. From the Draw menu select Edit Points
2. Select the contour.
3. Click and drag the contour points to move them.
4. Click and drag on the handles to change the shape.
5. To convert a curve into a line, right-click on the curve and select Convert to line.

Editing an Arc

1. From the Draw menu select Edit Points
2. Select the contour.
3. Click and drag the contour points to move them.
4. To change the curve of an arc, click on a point on the arc and drag it in or out.
5. To convert an arc into a line, right-click on the arc and select Convert to line.
6. To convert an arc into a curve, right-click on the arc and select Convert to curve.

Linear Curve Section Tool

Menu: Draw / Edit / Linearize

Toolbar: Contour Editing/ Edit Points / Linearize Curve Section

This tool allows you to edit a section of a contour. It will create a line between two points on the contour, allowing you to eliminate unneeded points quickly.
1. Click and hold the Edit Points Icon. This will open the flyout menu, click on the Linearize

Curve Section Icon

2. Click to place the first point on the contour.
3. Click to place the second point on the contour.
4. A pink line will appear to show the preview of the segment to be replaced.
5. Press the Enter key to accept the change.

Page 96 Contour Editing

Insert Corner

Menu: Draw / Edit / Cornet

Toolbar: Contour Editing/ Edit Points / Insert Corner

1. Click and hold the Edit Points Icon. This will open the flyout menu, click on the Insert

Corner icon. 

2. Click to place the first point.
3. Click to place the second point. This will show a preview of the new corner in pink. You can click on the second point and drag it to the desired location. The preview will reflect this change.
4. Press the Enter key to accept the change.

Smooth Approximation

Menu: Draw / Edit / Curve Fit

Toolbar: Contour Editing/ Edit Points / Smooth Approximation

1. Click and hold the Edit Points Icon. This will open the flyout menu, click on the Smooth

Approximation Tool Icon

2. Click on the contour to place the first point.
3. Click on the contour to place the second point. This will show a pink preview of the new segment. At this point you can adjust the new points and use the handles to change the shape of the new segment.
4. Once you get the new portion of the segment to look the way you want it, press the Enter
key to accept the change.

Noise Distortion

Menu: Transform / Distort / Noise Distortion 

Toolbar: Object Edit/ Scale/Distort / Add Noise to contours or Contour Editing / Edit Points / Add Noise to contours

One of the common criticisms of computer-aided designs, particularly for creative applications, is that the designs typically look “computer generated”. Everything is too precise and too perfect. Successful designers often create imperfections in their designs in order to make them look more natural. The Rapid Texture tool that was introduced in EnRoute 4 has been very successful at offering a method of creating surfaces that look natural, and therefore, interesting to the eye. The current EnRoute extends the ways that you can introduce “noise” into your designs by providing noise distortion tools for contours, toolpaths, and reliefs. By defining parameters, you can introduce distortions ranging from very small to dramatic. The goal is to provide creative tools that allow you to create effects that make

Contour Editing Page 97

your designs more interesting and more unique.
The following images show an example of changes that were made to the contours. This tool allows
the user to get an entirely different effect simply by adding a little “noise” to the contours.


The Noise Distortion tool can be used on both contours and relief surfaces. It provides two methods (1 and 2) for achieving the distortion. The first method provides fewer parameters, and can be considered the “simple” method.

Method 1

Wavelength

This defines the length along the contour over which the noise takes place. Larger values have the effect of spreading out the distortion over longer distances.

Jitter

This is a descriptive term for the parameter that controls the strength of the distortion. A small value such as 0.5 will create subtle distortions, while larger values will strengthen the distortion force.

Horizontal

Amplitude

This controls the “height” of the distortion in the horizontal (X-Y) plane.

Vertical Amplitude

This controls the distortion vertically. It may often be desirable to distort contours horizontally, but to keep them flat vertically. This would be true if you planned to use a Routing Offset to cut parts out of flat material. In that case the vertical amplitude would be 0.00.

Method 2

This method provides more parameters, so it might be considered the advanced distortion method; however, it is not really much more complicated than Method 1. There are two primary parameters, Size and Power, and there are two of each. The two set of parameters means that there are two distortion “passes” around the contours, and each pass is controlled by it parameters. By setting the

Page 98 Contour Editing

power parameters to 0.00 for a given pass, that pass won’t have any effect on the contours.

Size

This defines the size of the distortion in each of the three directions (X, Y and Z). You can think of this as sort of a combination of the Wavelength and Amplitude parameters from method 1. The interesting thing here is that you can define different parameters in different directions so that the distortion has a more directional result.

Power

This defines the strength of the distortion. Small values such as 0.02 allow you to create very subtle distortions of contours, and as the values increase the distortion becomes more dramatic. Since you can define parameters in all three directions, this is also a way to create a directional distortion.

The Distortion tool can be used to modify reliefs in addition to contours. Relief distortion can allow you to create effects that are quite different from the effects achievable by adding a relief to a distorted contour. The following graphic provides an illustration.

In this image, the contour on the left is the original contour. The second contour is the contour after it has been distorted. In this distortion you will notice that Method 2 provided the chance to modify the contour mostly in the x direction. The first relief is the result of adding a beveled relief to the distorted contour. The relief on the right was created by adding the beveled relief to the original contour and then applying the same distortion. You can see that the resulting relief is quite different, and the distortion of the contour and the relief seems more in synch. This is a fun tool to experiment with in order to create cool results.

Contour Editing Page 99


In the image above, the original relief on the left has been distorted to obtain the relief on the right. By distorting the relief, with subtle parameters, you see that it is easy to achieve a result that is interesting and that when cut out would have the appearance of having likely been created by hand rather than with a machine.

Extending Contours

Menu: Draw / Extend

Toolbar: Contour Editing / Extend

The Extend tool is used to extend an open contour either interactively, by a specific distance, or to an intersection with another contour. Line segments are extended with a straight line, Bezier segments are extended with a straight line that is tangent at the extension point, and Arcs are by default extended as arc segments. When extending the contour, arcs may also be extended as a straight line by holding down the Ctrl key while extending.

Extending a Contour Using the Mouse

Menu: Draw / Extend

Toolbar: Contour Editing / Extend / By Graphic

To extend an open contour using the mouse:
1. Click the Extend Icon This will open the Precision Toolbar. The Method – By

Graphic -is selected by default.

2. Click on the end of the contour you want to extend.

Page 100 Contour Editing

 As you move the cursor away from the end of the contour, a preview is provided to show the amount that the contour will be extended.

3. Move the cursor to the new endpoint and click.
4. After a contour has been extended, you can add another extension to the end of the extension.
5. Right-click to release the tool or click on the close button.
This option can work well with the Snap options to extend a contour to a specific point.

Extending a Contour by a Precise Length

Menu: Draw / Extend

Toolbar: Contour Editing / Extend / Precise Length

1. Click the Extend Lines Icon; this will open the Precision Toolbar.
2. In the Precision Toolbar select the By Length method and enter the length you want to extend contours by in the length field.
3. Click on the end of a contour to extend it by the specified amount.

 As you move the cursor over the end of an open contour, a preview of the extension is displayed.

4. After a contour has been extended, you can add another extension to the end of the extension.
5. Right-click to release the tool or click on the close button.

Extending a Contour to Boundaries

Menu: Draw / Extend

Toolbar: Contour Editing / Extend / Boundaries

To extend a contour until it intersects with another contour:
1. Click the Extend Lines Icon. This will open the Precision Toolbar.
2. Select the By Boundaries method.
3. Click on the contours you would like to use as boundaries.
4. To select all contours as boundaries, click on the All boundaries button.
5. To clear all selected boundaries, click on the Clear boundaries button.

Contour Editing Page 101

6. Click on the Extending button.
7. Click on the end of a contour to extend it to its intersection with the nearest boundary contour.

 As you move the cursor over the end of an open contour, a preview of the extension is displayed.

8. After a contour has been extended, you can add another extension to the end of the extension. This extension will go out the other side of the boundary, and proceed to the next intersection.
9. Right-click to release the tool or click on the close button.
If the Intersection box is checked, contours can be extended to the intersection with a line tangent to the end of a boundary. If the contour and the boundary are parallel, or if the end of the contour points away from the end of the boundary, no extension will be created. This can be helpful if you need to extend two contours so that they meet at their intersection.

Any open contour in the design can be extended. Even if a contour is selected as a boundary contour, it can still be extended to another boundary contour. This means that you can select all the contours in your design as boundary contours, and then proceed to identify which contours to extend.

Trimming Contours

Menu: Draw / Trim

Toolbar: Contour Editing / Trim

The Trim tool allows you to shorten a contour either interactively, by a specific distance, or based on intersections with boundary contours.

Trimming a Contour Using the Mouse

Menu: Draw / Trim

Toolbar: Contour Editing / Extend/Trim / By Graphic

1. Click and hold the Extend/Trim Line Icon then click the Trim Contours Icon
This will open the Precision Toolbar.
2. Select the By Graphic method.

Page 102 Contour Editing

3. Click on the end of the contour you want to trim.

 As you move the cursor away from the end of the contour, a preview is provided to show the amount that the contour will be trimmed.

4. Move the cursor to the new endpoint and click.
5. Repeat for as many contours as necessary.
6. Right-click to release the tool or click on the close button.
This option works with the snap options to trim a contour to a specific point.

Trimming a Contour by a Precise Length

Menu: Draw / Trim

Toolbar: Contour Editing / Extend/Trim / By Length

1. Click and hold the Extend/Trim Line Icon then click the Trim Contours Icon
This will open the Precision Toolbar.
2. Select By Length method and enter the length you want to trim contours by in the field.

 The length that is trimmed is determined by following the path of the contour from the end point, not as a radius or some other method.

3. Click on the end of a contour to shorten it by the specified amount.

 As you move the cursor over the end of a contour, a preview is provided to show the amount that the contour will be trimmed.

4. Repeat for as many contours as necessary.
5. Right-click to release the tool or click on the close button.

Contour Editing Page 103

Trimming a Contour to Boundaries

Menu: Draw / Trim

Toolbar: Contour Editing / Extend/Trim / By Boundaries

To trim a contour at the points where it intersects with another contour:
1. Click and hold the Extend/Trim Lines Icon then click on the Trim Contours Icon
2. In the Precision Toolbar, click on the By Boundaries method.
3. Click on the contours you would like to use as boundaries.
4. To select all contours as boundaries, click on the All boundaries button.
5. To clear all selected boundaries, click on the Clear boundaries button.
6. Click on the Trimming button.
7. Move cursor over the contour to be trimmed. A preview will highlight the part of the contour that will be trimmed. Left click on the mouse to activate the trim.


 As you move the cursor over the end of an open contour, a preview of the trimmed area is displayed.

8. Repeat for as many contours as necessary.
9. Right-click to release the tool or click on the close button.

Filleting Contours

Menu: Draw / Fillet

Toolbar: Contour Editing / Fillet

The fillet tool inserts an arc of a defined radius at selected corners of one or more contours.

Fillet Precision Toolbar

Page 104 Contour Editing

Single Fillet The single fillet allows you to select one specific corner to fillet.

Multiple Fillet This allows you to choose to Fillet All corners, Outside corners or Inside corners all at the same time with the same parameter.

Inside Corners  


Outside

Corners



All Corners

Radius This is the parameter for the size of the radius for the Fillet or Chamfer.

Chamfer Select this box if you would like to chamfer the corner instead of fillet.

Keep Original When this box is selected, the original will be kept and an open contour segment will be placed where the fillet was previewed.

Contour Editing Page 105

Single Fillet

Menu: Draw / Fillet

Toolbar: Contour Editing / Fillet / Single Fillet

1. Click the Fillet IconThis will open the Precision Toolbar.
2. Click the Single Fillet Icon
3. Select the first segment of the contour.
4. Select the second segment of the contour.
5. Enter in the radius dimension. This will show a preview of the fillet.
6. Click Apply.

Multiple Fillet

Menu: Draw / Fillet

Toolbar: Contour Editing / Fillet / Multiple Fillet

1. Click the Fillet Icon This will open the Precision Toolbar.
2. Click the Multiple Fillet Icon
3. Select the contour.
4. Choose one of the Corner parameters: All corners, Inside corners, or Outside corners.
5. Enter in the radius dimension. This will show a preview of the fillet.
6. Click Apply.

 Notice that where the fillets overlap, the software automatically makes them tangent with each other.

Page 106 Contour Editing

Joining Contours

Menu: Draw / Join

Toolbar: Contour Editing / Join

The Join tool allows you to join open contours to create larger contours.
1. Click on the Join Icon
2. Click on the end point of one of the contours you wish to connect.

 When you put the cursor over the end of a contour, the contour is highlighted.

3. Click on the end point of the second contour that you wish to connect.

 You will notice that EnRoute draws a red preview line between the two contours and highlights the second contour.


The joined contours are now one large contour.

Offset Contours

Menu: Draw / Offset Contours

Toolbar: Contour Editing / Offset Contours

This tool is used to create a contour that is offset from the selected contour.
1. Select the contour.
2. Click the Offset Icon. This will open the Precision Toolbar.

Contour Editing Page 107

3. Enter the number of Offset contours desired.
4. Enter the amount of the offset.
5. Select Outline or Inline.
6. Select Rounded or Square.
7. A preview of the Offset is shown on the screen.
8. Click Apply to accept.

Partial Offset Contours

Menu: Draw / Offset

Toolbar: Contour Editing / Offset Contours / Partial Offset


This tool is used to create a contour that is offset from the selected contour.

1.

Select the contour.

 

2.

Click and hold the Offset Icon then click the Partial Offset Icon. Precision Toolbar.

This will open the




3. Select the square or the rounded offset icon.
4. Click on the segment or segments that you wish to offset. Hold the shift key to select more than one segment at a time.
5. Enter the amount of the offset.
6. Click the mouse on the side of the segment that you want the offset to be placed.
7. Press Close to exit the tool.

Page 108 Contour Editing

Merging Selected Open Contours

Menu: Transform / Merge Selection

The Merge Selection tool is used to join open contours together based on a definable tolerance.

 This capability can be very useful if you are using contour information that has been generated in a different software package. Many CAD programs are oriented toward drafting functions, and don’t place an emphasis on closed contours as is necessary in order to create toolpaths . After importing a file into EnRoute, this tool provides a means of quickly joining separate contours into closed shapes that are more compatible with toolpath creation.

To join two or more open contours:
1. Select the open contours.
2. From the Transform menu, select Merge selection

3. Define the Merge Tolerance (the maximum distance endpoints can be separated by and still be connected).
4. Click OK.

Explode Selected Contours

Menu: Transform / Explode Selected Contours

This tool is used to separate a contour into individual segments. To explode a contour:
1. Select the contour.

Contour Editing Page 109


2. From the Transform menu, select Explode Selected Contours.
3. This will create individual segments for the contour.

Converting Curves to Arcs

Menu: Transform / Convert Curves to Arcs

The Convert Selection to Arcs tool transforms the contours in the selection, converting the lines and
Bezier curves into arcs.

 When a curve is converted to arcs, one curve may require several arcs, so the number of segments may increase significantly.



To convert contours into arcs:
1. Select the contours.
2. From the Transform menu, select Convert Selection to Arcs

Reverse Open Contours

Menu: Transform / Reverse open Contours

This tool reverses the direction of an open contour.
The direction of the contour is indicated by the direction of the arrow head on the contour. To display this option, go to the Setup MenuPreferences, View Setup and check the box for Open contour direction.
To reverse the direction of the contour:
1. Select the contour.
2. From the Transform menu select Reverse open contour
The example below shows that the arrow of the first line segment was pointed to the right. After it was selected and reversed, the arrow is showing to direction to the left.

Page 110 Contour Editing

Creating Multiple Copies of a Contour

Array Copy

Menu: Draw / Multicopy

Toolbar: Contour Editing / Multicopy

The Array Copy tool produces multiple copies of the selected contour, ordered into a specified number of rows and columns with a specified spacing.
For example, if you need to cut out several copies of the same contour, it is a simple task to create those copies at the desired spacing on the sheet using this tool.
1. Click on the Multicopy Icon.  This will open the Precision Toolbar.

2. Select Array Copy
3. In the Precision Toolbar, enter the number of rows and columns of copies desired, and the space between the rows and columns. A preview of the copies will be shown in pink.
 If you have one or more contours that must be copied so they fill up your whole piece of material. (For example a 4 x 8 sheet): Simply check the Fill Plate Box. The selected contours will be copied to fill the entire plate. You do not need to fill in the number of horizontal or vertical copies. The spacing between the contours is based on the spacing between the rows and columns that have been defined.
4. Click Apply to place the copies.

Contour Editing Page 111

 This is an example of an array copy to fill the plate, with .10 horizontal spacing and .10 vertical spacing.

Arc Copy

Menu: Draw / Multicopy

Toolbar: Contour Editing / Multicopy

The Arc Copy tool takes an existing contour or set of contours and creates a series of duplicates spaced out along the curve of an arc. The arc of copies that is created is defined by the radius and angle of the arc, the number of copies that are spaced along that angle, and the positioning point that will be used to position the copies on the arc.
1. Click the Multicopy Icon This will open the Precision Toolbar.
2. Select Arc Copy
3. Select the object to copy. A preview will show on the screen as you enter information into each of the parameters in the Precision Toolbar once you have selected the object to copy.
4. Enter the Number of copies that will be spaced along the arc.
5. Enter the Radius of the arc.
6. Enter the Start Angle (in degrees)This represents the point at which the arc begins.
7. Enter the Swept Angle, which defines the portion of a circle (in degrees) that will be used by the arc. If more than 360 degrees are entered, the arc will loop around.
8. Check Align to Path to rotate the copies along the curve of the arc.

Page 112 Contour Editing



Aligned Not Aligned
9. Click the reference grid button that corresponds to the corner, side or center point that will be used to position the contours along the arc.
These are the parameters used in the below example.


Object with positioning points

Preview of Arc Copy Result of Arc Copy

Contour Editing Page 113


The positioning point that is chosen can have a major effect on the appearance of the final set of copies. The examples below are all copies of the same right triangle, and use identical parameters apart from the positioning point selected.








Path Copy

Menu: Draw / Multicopy

Toolbar: Contour Editing / Multicopy

The Path Copy tool allows a shape to be copied along another contour by defining the number of copies, spacing, and how the contours are to be aligned.

1. Click Multicopy This will open the Precision Toolbar.
2. Select Path Copy
3. Select the object to copy. Then select a contour for the path by clicking on it. A preview will show on the screen as you enter information into each of the parameters in the Precision Toolbar.

Page 114 Contour Editing

4. Enter the Number of copies. The spacing will be adjusted accordingly.
5. Enter the Radius of the arc.
6. Enter the Offset Percentage. Use Offset if you want the original contour offset from the starting point of the path contour. The percentage is based on the spacing.
7. Check Align to Path to rotate the copies to match the direction of the path.
8. Select one of the following copy placement options:

Hold

Number

Enter the number of copies and the spacing will be calculated to keep them evenly spaced.

Hold

Spacing

Enter the desired spacing and the program will calculate how many copies will fit in the path.

All Corners

Copies will be placed at both inside and outside corners along the path.

Inside

Corners

Copies will be placed only at inside corners on the path.

Outside

Corners

Copies will be placed only at the outside corners on the path.

9. Click the reference grid button that corresponds to the corner, side or center point that will be used to position the contours along the arc.
10. Click Apply.

 The example below shows how to create a gear shape by first drawing a circle and a rectangle, and then copying the rectangle around the circle. The Weld Joined command is used to combine the shapes.


Contour Editing Page 115

Vectorizing Bitmaps

Menu: Draw / Vectorize Bitmap

Toolbar: Contour Editing / Vectorize Bitmap

Since the software uses vector-based contours to create toolpaths, any bitmap artwork you may want to use in your design must first be converted into a vector form. This technique is called vectorization.
The Vectorize Bitmap tool allows you to trace bitmap art and convert it into contours.

 Before vectorizing a bitmap, you should clean up the bitmap as much as possible using a bitmap editor. Remove specking and unwanted detail. Make sure that contours you want to turn into closed contours are completely closed in the bitmap. If possible, convert the image to a grayscale or black and white image.

1. Import the bitmap into your design and select it.

 For information on importing a bitmap or other graphic, see “Importing a Design “.

2. Select Vectorize bitmap

In the Vectorize dialog, select the BezierEnhanced corners, or Enhanced curves option.
 The Bezier option emphasizes using Bezier curves as it completes the vectorization process.
 The Enhanced Corners option emphasizes creating a contour with distinct sharp corners. It also provides a number of additional parameters that affect the vectorization process.
 The Enhanced Curves option emphasizes using arcs to provide a best fit of the vectors to the original artwork.

Page 116 Contour Editing

3. Check the Auto cleanup box if you want the software to attempt to automatically simplify the contours it creates. Set Tolerance to the size of the smallest features on the bitmap that you want the software to keep. See “Cleaning Up Contours” for details.

Cleaning Up Contours

Menu: Draw / Cleanup

Toolbar: Contour Editing / Cleanup selected contours

The Cleanup tool automatically simplifies the selected contours so that they use fewer segments to achieve the same effect. This makes it easier for the software to create toolpaths, and reduces the chances for the toolpath creation process to fail because of some odd configuration in the geometry.


304 Segments 65 Segments
1. Select the contour.
2. Select Cleanup
3. Set Tolerance to the size in inches of the smallest features you want the software to keep.

Contour Editing Page 117

4. Higher Tolerance settings will cause the contour to be simplified more, but they will also change the appearance of the contour more.
5. Click OK.

Page 118 Contour Editing

7. Arranging Contours

Selecting Contours

To select a contour, click on its edge.
You can also select multiple contours using one of the following methods:
 Hold down the SHIFT key and click on the contours one after the other.

 Click and drag to draw a selection box around the contours.

 From the Edit menu, select Select All to select all contours in the current design.

Automatic Sorting for Open Curves, Containers and Holes

Whenever one or more contours are selected, the software automatically checks to see whether the contours are open curves, containers or holes.
By default, all closed curves are classified as containers.
If a closed contour is completely contained within another closed contour, the outside contour is identified as a container, and the inside contour is identified as a hole in that container. The contour of the hole forms an inner edge to the container contour.
The following illustration shows two contours being selected, converted to a container and hole, and being filled with a Hatch Fill toolpath.





By default, open curves are color-coded purple, containers are color-coded blue, and holes are color- coded red.

Cutting, Copying and Pasting Contours

Menu: Edit / Cut or Paste

Toolbar: File / Cut or Paste

To cut and paste contours:
1. Select the contours to cut.

Arranging Contours Page 119


2. From the Edit menu choose Cut or press Ctrl+X.
3. Select the design where the contours are to be pasted.
4. From the Edit menu choose Paste or press Ctrl+V

 When there is more than one design window open, use the Cut and Paste commands to remove a group from one design and place it in another. You can continue to paste the cut selection until something else is placed onto the Clipboard.

Copying and Pasting

Menu: Edit / Copy or Paste

Toolbar: File / Copy or Paste

1. Select the contours to copy.
2. From the Edit menu select Copy or press Ctrl+C
3. If the copied image is to be pasted into a different design, select the design where the contours are to be pasted.
4. From the Edit menu select Paste or press Ctrl+V

 When pasting into the same design, the copied image will be placed in the same place as the original. Move the original image to the new location before pasting.

 If you want to make a copy within the same design, press the CTRL key, click on the center control box and drag a copy to a new location.

Pasting from Other Programs

See the Preference command located in the Setup menu for options regarding Merge Contours and
Automatic Cleanup.

Deleting Contours

Menu: Edit / Delete

Toolbar: File / Delete


1. Select the contours.
2. From the Edit menu, select Delete.

Page 120 Arranging Contours

 You may also select the contours to be deleted and press the Delete key instead of selecting the

Delete command.

Grouping and Ungrouping Contours

Menu: Transform / Group or Ungroup

Toolbar: Object Edit / Group or Ungroup

Grouping contours together allows you to select and manipulate a group of contours as a single contour. After grouping contours together, you can also Ungroup them to return them to their original state. This tool is used mainly as a convenience when you are working on intricate designs.

1. After creating a number of contours, select them.

 Notice that the contours are automatically sorted when they are selected.

2. Click on the Group Icon
 After selecting the contours, you want to group you can press Ctrl+G to group them.

Now, when you change the size of the group, or move it around, it will be treated as a single object.
If you select any part of the group to work with, you will be selecting the entire group. You can use the control points, or handles, to scale the entire group as a unit.
 To separate the group into its component contours, simply select the group and click on the Ungroup Icon, or press Ctrl+U

Moving, Scaling, and Rotating Objects

EnRoute provides several methods for interactively and precisely moving, scaling and rotating objects. It is important to be able to quickly move and scale objects in the drawing, but it is equally important to be able to position and size objects very precisely. EnRoute’s tools meet both of these needs.

Arranging Contours Page 121

Moving and Scaling Interactively

Within EnRoute’s standard interface it is possible to move and scale objects simply by selecting them and clicking and dragging. For creative design work that doesn’t necessarily require precise placement or sizing, this is the easiest and quickest method.
In order to move a selection, it is as easy as clicking on one of the contours in the selection and then dragging the selection to a new location. It is important, though, to click on one of the selected contours in order to maintain the selection. The image below illustrates this – note that the cursor is on top of one of the contours in the selection.

It is also possible to move a selection using one of the nine selection handles. The easiest way is to place the cursor on the center handle and then click and drag the selection to a new location. It is also possible to move a selection using one of the other handles but this takes a little practice. If you place the cursor directly on top of one of the handles, notice that the center of the cursor arrow turns black. If you click and drag at this point, you will scale the selection rather than move it.

 Vs. 

If, instead of placing the cursor directly on top of the handle you place the cursor near the handle and then click and drag, the selected point for the move will automatically snap to the corner of the selection and then allow you to move the selection to the desired location. After you master the concept of clicking near a corner this is a handy way to precisely position a selection.
Scaling a selection interactively is accomplished by placing the cursor on one of the selection handles and then clicking and dragging to move the handle and scale the selection. If you also press the Shift key while dragging the handle the selection will be scaled proportionately.

Page 122 Arranging Contours

Moving, Scaling and Rotating using the Precision Input Center

The Precision Input Center has been used in EnRoute historically as the method for precisely locating objects. Although new tools are now available for accomplishing these tasks, the Precision Input Center is still available for this purpose. One of its advantages is that it provides a simple method for precisely sizing and locating objects.

The Precision Input Center is activated by pressing the F2 key. The selection can be scaled by entering values either for Dimensions or Scale Factor. In order to proportionally scale the selection, make sure that the Proportional checkbox is checked. Click on the OK button in order to complete the scaling activity.
Rotating the selection using the Precision Input Center is similar to scaling. After selecting the objects to be rotated and activating the Precision Input Center, click on the Rotate tab. The rotation axis will be based on the active viewport. From the top view you will typically rotate the selection about the Z axis. This means that the objects are rotated in the X-Y plane. Enter the desired rotation angle and click on the OK button to complete the rotation. The center of rotation defaults to the center of the selection; however, it can be placed to a different location if desired.

Arranging Contours Page 123


In order to Move the selection, click on the Move tab, select the corner of the selection for which you want to specify the location, and then enter the coordinates for that location. Click on the OK button to execute the move.

When specifying the corner of the selection to move, the active viewport defines which plane is active. In the top view, the X-Y plane is active and the corner points are located on the plane nearest the viewer. For reliefs, this means that the points are located on the top of the relief. In the front view, the corner points are located on the X-Z plane on the side of the object closest to the viewer.
Note: The Include Toolpaths checkbox lets you choose whether toolpaths are included in the size and location coordinates for the selection.

Move, Scale, Rotate Tools

EnRoute also includes tools for moving, scaling, and rotating objects that are quite flexible and that provide a number of options for accomplishing these edits. These tools are accessed from the Object Edit toolbar and the Transform menu item. Additionally, you can move between these functions from within the Move-Scale-Rotate toolbar after it has been activated. A graphic of this toolbar is shown below.

The following sections provide a detailed description of the parameters for each of the tools and also provide some step-by-step direction.

Page 124 Arranging Contours

Move Tool

Menu: Transform / Move

Toolbar: Object Edit / Move

The Move tool provides three different methods for moving selected objects. Within each of these methods you have the option of either entering coordinate information to define locations or defining locations interactively in the drawing.

Move Absolute 

The Move Absolute method allows you to define a starting point and ending point for the move. Objects can be positioned very precisely by defining locations for the move based on entered coordinates. With the point snap options, it is also an easy task to position the selection precisely by clicking in the drawing.

Move Relative 

This method is similar to the absolute method, with the exception that it allows you to define the amount of the move in each direction. Use it to move the selection over 5 and up 3.

Move Corner 

Use this method to position a selected corner to a specific point. It is an easy way to move the lower-left corner of the selection to a specific point.

Start

In the Absolute mode this is the coordinate of the start of the move operation.

End

In the Absolute mode this is the coordinate of the end of the move operation.

Origin

In the Relative mode this is the coordinate of the start of the move operation.

Move

In the Relative mode this is the amount of the move in each direction.

Copy

By checking this checkbox, you can create a copy of the selection when it is moved. The original will stay in place.

Corner Selector

In the Corner mode this lets you choose which corner of the selection for which to specify a new location.

To Move a selection:
1. Select the objects to be moved.
2. Click on the Move Iconselect it from the Transform menu or press Shift+F5. This will activate the Precision toolbar for the Move tool.

Arranging Contours Page 125


3. Choose the desired move Mode. In this case choose Move Absolute.

4. Define the coordinate of the start point of the move. This can be done by typing in the coordinate values or by interactively clicking on a start point.
5. Define the end point of the move by typing in the end point coordinate or by clicking on the end point in the drawing.
6. If you click on the end point, then the move will be completed. If you define the coordinate of the end point, then click on the Apply button to complete the move.

Key Concept with Right Click – The right-click button on the mouse can be used to ‘back out’ of the Move-Scale-Rotate tools. When you right click while you are in the tool, the effect will be to back you up one step. For example, in the image above the user has selected the objects to be moved, clicked on the start point for the move and is in the process of locating the point for the end point of the move. A right click at this point would back the user to the point of defining the start point of the move. Another right click would deselect the two rectangles. Another right click would exit the move tool.

Scale Tool

Menu: Transform / Scale

Toolbar: Object Edit / Scale


The Scale tool provides several options for scaling selected objects. For scaling interactively, the scale tool uses a reference line to define the base point of the scale and the scale factor. The tool

Page 126 Arranging Contours

also allows you to enter a precise size or scale factor for the scaling operation.

Scale Three

Dimensions

When the selection is scaled, it will be scaled in all three dimensions regardless of what view is active. This applies mostly to three- dimensional objects such as Reliefs and Meshes.

Scale Two

Dimensions

When the selection is scaled, only the two visible dimensions will be scaled. In the Top View only the X and Y dimensions will be scaled. This is helpful when scaling a Relief when you don’t want the thickness of the relief to change.

Scale One

Dimension

When the selection is scaled interactively using the reference line, it will be scaled along the direction of the reference line. This will have the effect of distorting the scaled objects in the direction of the reference line. If the reference line is defined either horizontal or vertical, then the scaling will be along the X or Y axis. This option will likely be used less often than the other two scaling options as more of a specialty tool.

Size

Precisely scale the selection by entering the desired XYZ size.

Factor

Precisely scale the selection by entering the scale factor.

Include Toolpaths

Include any toolpaths in the selection in the Size parameter.

Proportional

If checked, any scaling operation will be performed proportionally to the selection.

Copy

By checking this checkbox, you can create a copy of the selection when it is scaled. The original will stay in place.

Corner Selector

This selector is used when Size or Factor parameters are used to scale the selection.

To Scale a selection precisely:
1. Select the objects to be scaled.
2. Click on the Scale Icon select it from the Transform menu, or press Shift+F6.
3. Choose the scaling option you prefer. In this case, choose Scale Three

Dimensions

4. If you want the scale operation to be proportional, make sure this checkbox is checked.
5. If you want to make a copy of the selection, make sure this checkbox is checked.
6. Enter either the desired Size or Scale Factor.
7. Choose the desired corner to serve as the anchor point for the scaling operation.

Arranging Contours Page 127

8. Click on the Apply button to perform the scaling operation.
To Scale a selection interactively:
1. Select the objects to be scaled.
2. Click on the Scale Icon select it from the Transform menu, or press Shift+F6.
3. Choose the scaling option you prefer. In this case choose Scale Two

Dimensions

4. Click on the point you would like as the anchor point for the scaling operation. This can be a specific point if you would like the selection to remain in a specific location, or it can be any point on the screen if the location is not important. This point is the start point of the reference line.
5. Click on another point that will serve as the end point of the reference line. Again, this point can be a specific point so that the reference line is a specific length, or it can be any point in the view.
6. The next point defines the length of the scaling line. The scale factor for the scaling operation is based on the proportional length of the reference line relative to the scaling line. Both lengths are defined from the anchor point. After the scaling line is defined then the scaling operation is completed.
The following graphic illustrates how the Reference Line and Scaling Line lengths are used to determine the Scale Factor.

Page 128 Arranging Contours

L1 - Reference Line

L2 - Scaling Line

Scale Factor = L2 / L1



Using the Scale One Dimension option will scale the selected objects along the reference line. If the reference line is drawn horizontal, then the scaling will be done along the X axis. If the reference line is drawn vertical, then the scaling will be done along the Y axis. If the reference line is drawn at some other angle, then the selection will be distorted along the line. The following images show one- dimensional scaling along the X axis and along another line.

Arranging Contours Page 129

Scaling along the X Axis

Scaling along an arbitrary line

Rotate Tool

Menu: Transform / Rotate

Toolbar: Object Edit / Rotate

The Rotate tool allows you to rotate selected objects both precisely using a defined rotation center point and a rotation angle, and interactively by defining a rotation center, a starting direction, and a finished direction. You can also choose to perform the rotation using a combination of interactive and precise input.
Following is a definition of the elements of the Rotate toolbar:

Center

This allows the rotation center to be defined precisely.

Axis

This is the axis about which the rotation will be completed. In the top view the axis will most often be defined as the Z axis.

Angle

This is the rotation angle.

Copy

If this is checked then the rotated objects will be a copy of the originals.

Page 130 Arranging Contours

Corner Selector This defines the location of the rotation center when rotating the selection using the Angle parameter in the toolbar.


To Rotate a selection precisely:
1. Select the objects to be rotated.
2. Click on the Rotate Iconselect it from the Transform menu, or press Shift+F7.
3. Enter values for the Center of rotation or select the desired corner from the Corner Selector.
4. If you want to make a copy of the selection, make sure this checkbox is checked.
5. Enter the Angle.
6. Click on the Apply button to perform the rotation. To Rotate a selection interactively:
1. Select the objects to be rotated.
2. Click on the Rotate Iconselect it from the Transform menu, or press Shift+F7.
3. Click on a point to define it as the Center of rotation.
4. Click on another point to define the initial direction. The line between the first clicked point and the second clicked point defines the “zero” direction for the rotation. As you move the mouse around you will see a preview of the rotation.
5. Click on a point to define the angle of rotation and to complete the rotation.

Arranging Contours Page 131


The first click defines the center of rotation and then the second click defines the reference line for the rotation.

Moving the mouse provides a preview of the rotation. The third click defines the angle and completes the rotation.

Page 132 Arranging Contours

Distort Contours

Menu: Transform / Distort

Toolbar: Object Edit / Scale / Taper Distort

The Distort tool allows you to stretch an object disproportionately.
1. Select the contour.
2. Click and hold the Scale Icon then click the Distort Tool
3. Click on one of the external selection handles and drag the mouse to the desired position.
4. Press Enter to accept the change.
5. Right Click to end the tool.

Patch Distort

Menu: Transform / Distort / Patch Distort

Toolbar: Object Edit/ Scale/Patch Distort

External Selection Handle

This tool distorts selected contours or reliefs by defining a “patch”, or grid, or control points. By moving the control points either together or separately, you can introduce distortion into the selection. This allows you to modify your selection to fit a specific path or shape.
1. Select the relief and click and hold the Scale Iconand then click on the Patch Distort

Icon. 

Arranging Contours Page 133

2. A grid will be placed over the relief. Click on one or more selection points and drag to desired location.


3. This example shows the center selection points were moved.
4. Click Enter to apply the change.

5. Right click to end the tool.

Page 134 Arranging Contours

Mirroring a Contour

Menu: Transform / Mirror

Toolbar: Object Edit / Mirror

This tool reverses the selected contour so that it becomes its mirror image. This can be done interactively by defining the axis around which to create the mirror, or simply clicking on the horizontal or vertical tools. You can choose to create a copy of the object as well.

Mirror Dialog

Click the Mirror Icon.  This will open the Precision Toolbar.

Mirror Interactively

1. Click the Mirror Line Icon
2. Select the object or objects that you wish to mirror.
3. Simply click to place the start point of the axis and click again to place the end point. The axis can also be defined by entering the parameters for the start point and the end point of the axis line. A preview of the mirrored object will show on the screen as you are working to place your object.

Without checking the copy box the reversed 4 will be the end result.

If you check the copy box, you will still have the original object as well as a reversed copy.

Arranging Contours Page 135

Mirror Horizontal

Menu: Transform / Mirror

Toolbar: Object Edit / Mirror

1. Click the Mirror Icon. This will open the Precision Toolbar.

2. Select the object or objects that you wish to mirror.
3. Click the Mirror Horizontal Icon A preview of the mirrored objects will show in pink.
4. Click the reference grid button that corresponds to side or center point that will be used to locate the mirrored object.






5. Click Apply to accept.

Without checking the copy box the reversed 4 will be the end result.

If you check the copy box, you will still have the original object as well as a reversed copy.

Page 136 Arranging Contours

Mirror Vertical

Menu: Transform / Mirror

Toolbar: Object Edit / Mirror

1. Click the Mirror Icon. This will open the Precision Toolbar.

2. Select the object or objects that you wish to mirror.
3. Click on the Mirror Vertical Icon A preview of the mirrored objects will show in pink.
4. Click the reference grid button that corresponds to side or center point that will be used to locate the mirrored object.






5. Click Apply to accept.

Without checking the copy box the reversed 4 will be the end result.

If you check the copy box, you will still have the original object as well as a reversed copy.

Arranging Contours Page 137

Aligning Objects Menu: Transform / Align Toolbar: Object Edit / Align

The Align tool allows you to align one or more EnRoute objects relative to each other.
1. Select the objects to be aligned.
2. Click and hold the Align Icon, then click one of the following:


Alignment [to horizontal &

vertical center] 







Align to bottom   Align to top   Align to center

vertically





Align to center horizontally


Align left  

Page 138 Arranging Contours



Align right

Welding Contours Menu: Transform / Weld Toolbar: Object Edit / Weld

All of the Weld tools work by combining multiple contours into one. Each tool yields different effects,
however, due to the way in which the volumes of the contours are combined.

Using the Weld Joined tool

Menu: Transform / Weld / Weld Joined

Toolbar: Object Edit / Weld / Weld Joined

The Weld Joined tool combines multiple contours into one contour. Overlapping areas are merged together to form a contour that is the union of the volumes of all its parts.



To weld contours together using the Weld Joined tool:
1. Select the contours to be welded together.
2. Click Weld joined

Weld Common

Menu: Transform / Weld / Weld Common

Toolbar: Object Edit / Weld / Weld Common

The Weld Common tool combines multiple overlapping contours into one contour that is the intersection of the volumes of the contours.

Arranging Contours Page 139




To weld contours together using the Weld Common tool:
1. Select the contours to be combined.
2. Click and hold Weld then click Weld Common

Weld Subtract

Menu: Transform / Weld / Weld Subtract

Toolbar: Object Edit / Weld / Weld Subtract

The Weld Subtract tool subtracts the volume of a number of contours from the volume of the first contour selected. The result is the first contour, minus any areas which overlapped with the other contours.



To weld contours together using the Weld Subtract tool:
1. Select the contour you want to subtract from.
2. Select the other contours to subtract from the first.
3. Click and hold Weld then Weld Subtract

Page 140 Arranging Contours

Weld Jigsaw

Menu: Transform / Weld / Weld Jigsaw

Toolbar: Object Edit / Weld / Weld Jigsaw

The Weld Jigsaw tool allows you to create shapes based on the intersections of contours in your design.
After activating the Jigsaw tool, you can move the cursor over the contours in your design and the software will outline closed shapes that it might create. It is okay for contours to be located at different points vertically. For the use of this tool, contours are projected down to a zero height in the Z axis, and the resulting jigsaw contour is created a Z = 0.0 in the X-Y plane.

When you find the closed shape you want, just click in the shape and that closed contour will be created in place in the design. You can then drag to the shape away from the existing contours.

 Note in the example above that the Jigsaw tool works with any type of graphic in the design, including both closed and open contours. This can be very useful when constructing closed shapes for toolpathing. The traditional CAD method of construction would require constructing lines and curves and then trimming them at intersection points, followed by joining them to create a closed shape. That method still works, but the Jigsaw tool can often get to the same result in fewer steps.

1. Click and hold Weld  then click Weld Jigsaw
2. Move the cursor over your design to see the contours that can be created by the tool.
3. To create a contour from one of the highlighted outlines, click on the design and drag the new contour away.
4. Right-click to release the Weld Jigsaw tool.

Arranging Contours Page 141

Using the Cut by Line Tool Menu: Transform / Weld / Cut by Line Toolbar: Object Edit / Weld / Cut by Line

The Cut by Line tool allows you to cut closed contours into multiple closed contours.



1. Click Weld  then click Cut by line
2. Click and drag to create your cutting line.
3. Right-click to release the tool.
The Cut by Line tool operates differently when used on multiple contours that are selected. This is because when you select a group of contours they are automatically grouped into containers and holes. When you use the Cut by Line tool, this grouping is respected. The following images show two contours that are cut, first without being selected, and second while selected. The first example creates four separate contours, while the second example creates just two new contours.






Page 142 Arranging Contours

Nest Tool

Menu: Transform / Nest / Nest

Toolbar: Object Edit / Nest / Nest

Nesting in EnRoute has been redesigned in order to do a better job of centralizing the nesting tools location, to implement several new capabilities, and to hopefully simplify the whole nesting process. The follow major changes were implemented.

 Two new nesting algorithms were implemented, providing several new nesting options.

 Contours can be automatically created that represent sheet remnants. These can then be used for nesting, allowing you to more easily utilize your material.

 Nesting obstruction can be specified, making it simple to nest around clamps or bad sections of material.

 A new block nester improves nesting of rectangles.

 Common-line cutting contours can be generated, allowing for efficient cutting of rectangles.

 A new Nesting Summary can be created to provide information about nesting results.

From the nest flyout tool you may access the Nest Dialog, the Dynamic Nesting Tool and the Nesting
Summary Report.

Nest Dialog

There are two different dialogs that can be accessed when the Nest Icon is selected. Each dialog will show which options are available to that specific nester, and some of them are available to both nesters. A short explanation of all of the options is listed below.

Shape Nester Dialog

Shape Nesting – This will open the dialog for the Shape Nester. This dialog incorporates many different options for nesting into one central area.

Nester Types:

Within the Shape Nester, there are 3 different types of nesters that can be used: StandardNew and Legacy. Each nester

Arranging Contours Page 143


uses a different algorithm to decide how the objects will be nested. Click on the nester name to highlight the chosen nester and to see which options are available with that nester. A short explanation of each nester is listed below.

Standard – The Standard Nester is the nester that most current EnRoute 4 users are familiar with.

New – This nester allows EnRoute to automatically recognize contours that are selected as nesting “obstructions” and will nest around these obstructions. This provides a very simple way to avoid clamps on the machine or to avoid a section of the material that is not good for nesting, such as knots or other defects in a solid wood panel.

Legacy – This is the original nester that was used with previous versions of EnRoute.

Block Nester Dialog

Block Nesting – The Block Nester is designed to be used with squares and rectangles. It can be the most efficient and fastest method of nesting. It allows for the option to create a common-line contour. This option is useful for cutting rectangular parts because it prevents “double cutting” of the parts.

Quantity - The number of copies that you wish to create and then nest.

Example: The user can assign the number of copies to all of the objects at once, or as shown in this example each object individually. Select the object and change the quantity to number of copies of that object you wish to create.
Continue by selecting the next object and entering the quantity you want to create for this one. Once you have assigned the quantity for each object, click Apply.

Priority Order - Enter the number of the priority for each object to be nested to determine the order it is to be nested.

Page 144 Arranging Contours

Gap - The minimum distance between each of the contours being nested.

Margin - The minimum distance between the edge of the plate and the contours being nested.

Nest Originals - When this box is checked the original objects will also be nested. When additional quantities have been created, the original objects will be highlighted when nested.

Multiple Sheets - When this box is checked, additional layers will be created to allow for the nesting of all selected objects. All of the nested layers will be turned on. It will show all of the layers displayed immediately after nesting. Click on the arrows in the Layers toolbar to display each layer individually and to choose one layer to be active.

Create Remnant - When this is checked a contour will be created that represents the remnant of the sheet of material used to cut the objects. The remnant can then be selected and a new plate can be created with that geometry.

Example:
Select the remnant contour and click on the  Create Plate from Selected Contour.

Create Summary - A summary report will be generated if the option is checked.

Step Angle - When using the Shape nester, this option allows you to specify the angle in degrees that the objects are allowed to rotate when nesting.

Allow Rotate - This allows the objects to rotate when using the Block nester.

Create Common Line - When using the Block nesting tool, users can choose to create a contour that can be used for common-line cutting. This is useful for cutting rectangular parts because it prevents “double cutting” of the parts.

Example: This is an example of the common line cutting feature.
1. Select the objects to be nested and click on the Nest Icon. This will open the nest dialog.
2. Click on the Block nesting icon. This will change the dialog to present only the options that are available to the block nester.
3. In this example, we changed the Quantity to 2 while all of the objects were selected. This will nest 2 of each object. The Gap is set at .25 because we will be using a ¼ inch tool to cut the pieces.
4. Select the Create common line checkbox.
5. Click Apply.

Arranging Contours Page 145


This image shows how the objects were nested, and that there are 2 of each object. The common line has also been created.

6. The next step is to apply an Open Contour Routing Offset to the common line contours.
7. Select the common line contour.

Page 146 Arranging Contours


8. Click and hold the Routing Offset Icon, and then click on the Router Offset Open

Contour  tool. This will open the Open Contour Offset dialog.


9. Select a ¼ inch end mill tool. In the parameters section select follow middle of the contour.
Click OK to apply the toolpaths.
This image shows the toolpaths that have been created. The second image is highlighted to show the width of the tool. By assigning the gap distance the same width as the tool, you cut both sides of adjacent parts at once.


Arranging Contours Page 147

Use Holes - If this option is selected, the software will place smaller contours within the holes in larger contours. This option is available with the Shape nester

Obstruct - When using the Shape nester and the New nester option, check this box and EnRoute has the ability to recognize areas of the sheet that you do not want used for the nesting. Contours will need to be placed in the area of the workspace and selected along with the nested objects when accessing the tool. This provides a very simple way to avoid clamps on the machine, or to avoid a section of the material that is not good for nesting, such as knots or other defects in a solid wood panel.

Example: This is an example demonstrating the obstruct option.
1. Create contours that represent the clamps or areas of the material that you do not want the objects to be placed when nesting.

2. Select all of the objects (the objects to be nested and the obstruction objects) Click on the nest icon to open the dialog. The obstruction objects will show in red.

3. Enter the options you would like for this nesting and be sure to check the Obstruct box.

Page 148 Arranging Contours

4. The contours are nested in the workspace avoiding all of the obstructions that you have created on the plate.

Reference Grid - Click on the button that represents the position of the plate that you want the

nested items to be located. With the New nester checked, you now have the choice of more than one
area of the material.

Nest Summary Report

The Nest Summary Report contains the following information:

Arranging Contours Page 149

The next section of the report contains is a reference of the parts nested.

The following section of the report shows a picture of the nested sheets and the individual data for each of the sheets.



Page 150 Arranging Contours

In this example two sheets were needed to nest the objects. The information for this sheet is shown here.


Dynamic Nesting Tool

Menu: Transform / Nest / Dynamic Nest

Toolbar: Object Edit / Nest/ Dynamic Nest

The Dynamic Nesting tool allows the user to drag objects onto the plate and have them automatically rotate to fit within the constraints of other objects and the edge of the plate. Several parameters allow you to adjust offsets and rotation steps.
1. Click and hold Nest and then Dynamic Nest

Arranging Contours Page 151

2. Left click to select the object. It will turn pink.

3. Left click to move the object into position. While you are dragging the object it will turn in several directions as you locate the area best to nest this object.
4. Left click to place the object.
5. Right click to release the object. You can now select another object to nest in the same manner or you can right click again to exit the tool.

Dynamic Nest Precision Toolbar

Menu: Transform / Nest / Dynamic Nest

Toolbar: Object Edit / Nest/ Dynamic Nest

1. Click and hold Nest and then Dynamic Nest
2. Press the F2 button to open the Precision Toolbar. Once you set these parameters they will not change until you open the Precision Toolbar to change them.

Rotation Steps – The rotation steps refer to the highest number of positions you allow EnRoute to try before placing the object.

Nest Resolution – The higher this number is the longer it will take to nest the object and the object will show more clearly.

Part Offset – The minimum distance between each of the contours being nested.

Plate Margin - The minimum distance between the edge of the plate and the contours being nested.

Page 152 Arranging Contours

8. Working with Toolpaths


The goal of the design process is creating toolpaths and then machining finished pieces. This chapter provides a detailed explanation of each of the different ways to create toolpaths.

Overview

Contours and Toolpaths

Toolpaths derive their shapes from the contours in your design. The contours may form the boundaries of the toolpath, as with a fill, or the toolpath may trace inside, outside or along the path of the contour.
While contours may contain Bezier curves, toolpaths are composed exclusively of arcs and straight line segments, in order to be compatible with the movements of tools in the routers, engravers and other and CNC devices which are used with EnRoute. Any Bezier curves which may be present in a contour are replaced (temporarily, and for the purpose of toolpath creation) by a combination of straight lines and arcs in the toolpath.

Toolpath Groups

When a toolpath is generated from a contour, both the toolpath and the original contour are grouped together into a toolpath group. If additional toolpaths are created based on the same contour, they will be added to the same toolpath group.
Each contour can belong to one and only one toolpath group. If you want to generate a toolpath based on a contour by itself, and a different toolpath based on a group of contours which includes the first contour, you will need to make two copies of the contour: one to use by itself, and one to use as part of the group.

 When this is necessary, it is helpful to keep the individual contour and the group of contours on separate layers in order to avoid confusion.

Strategy

When creating a toolpath, you must choose a strategy which determines the type of toolpath the software will generate (fill, engraving, slot, etc.). Each strategy has its own set of parameters which define virtually every aspect of the toolpaths that are created, such as tool type, depth, overlap, direction and speeds.
Because the strategy completely determines the appearance and shape of the final toolpath, the software always refers to the toolpath by the strategy that was chosen, not as a toolpath.

Plan

The plan is the set of all of the different strategies contained in any one toolpath group.

Working with Toolpaths Page 153

Cuts

Each toolpath strategy is made up of one or more cuts. For instance, a fill might have a Rough cut, a Fine cut, and a Clean cut. Each cut uses one specific tool, as well as the parameters associated with the type of cut it will be making.

Plan, Strategy and Cut Templates

At each step in the toolpath creation process, it is possible to define and save a library of templates that can be used to automate the process.

 A cut template saves the parameters associated with a single cut.

 A strategy template saves the parameters associated with a strategy, including the parameters of each of the cuts that make up the strategy.

 A plan template saves all of the parameters associated with all of the strategies for a given toolpath group, as well as the parameters for each of the cuts in each of the strategies.

The information saved in the templates can then be easily selected and reapplied to a different contour, recreating all the work that was done on the original toolpath group in one powerful step.
For example, a common activity is to create male and female routing offsets to be used to cut out different materials so that one may be inlayed into another. Both sets of toolpaths can be created based on one set of contours, and then selectively used to cut out the material. After determining the best combination of parameters for both types of offsets, they can be saved as a plan template so that these parameters may be recalled and reapplied at any time.

Creating Routing Offset Toolpaths

Menu: Toolpath / Routing Offset

Toolbar: Toolpath / Routing Offset

 The Routing Offset strategy can only be used with closed contours.

The Routing Offset strategy creates a toolpath that runs either inside or outside the selected closed contour. The toolpath is offset from the contour by the radius of the cutting tool, so that it will trim right up to the edge of the contour.



If the cutting tool cannot fit into a corner or tight curve of the contour, the toolpath will follow the closest smooth curve possible.

Page 154 Working with Toolpaths


To create a toolpath using the Routing Offset strategy:
1. Select the contour you want the toolpath to follow.
2. Click Routing Offset
3. In the Routing Offset dialog, select the desired tool from the Available Tools list and click

Add Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

 The first tool in the list is always defined as the Rough tool, and it is typically used as the main cutting tool. Any additional tools serve as Clean or Fine tools, primarily used as a final pass to clean up cutting marks from the Rough tool, or to fit into areas that the Rough tool couldn’t.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.
6. Set the Router Offset parameters:

External

(male)

Internal

(female)

If checked, the toolpaths will follow the outside of the contour.



If checked, the toolpaths will follow the inside of the contour.

Working with Toolpaths Page 155



Weld offsets If checked, overlapping offsets will be welded together to form a single toolpath group. If cleared, overlapping offsets will be left the way they are.

Sharp corners

When toolpaths are offset from square corners, they are naturally rounded. This does not affect the ‘squareness’ of the corner and it generally allows for smoother movement of the machine. If this option is checked, the toolpath offsets form square corners. It is generally not recommended to choose this option.

Inlay If checked, the toolpath defines either the socket for an inlaid piece of a different material (if the toolpath is set to Internal), or the cut that will separate the inlay itself from the plate (if the toolpath is set to External).

 Because a round bit is being used to cut out both pieces, both the male and female toolpaths need to take into account the dimension of the tool. This changes the shape of the toolpath, particularly in corners.

If this option is checked, the Inlay Gap parameter displays. This parameter indicates the size of the gap that will exist between the inlay and its socket.

With Bridges Bridges are small tabs of material that are left connecting parts which would otherwise be completely severed from the rest of the design. After the job has finished cutting, the operator can then manually cut the bridges to remove the part from the rest of the plate.

If this box is checked, bridges will be created.
If the With Bridges option is checked, other parameters are activated to allow the user to enter the number, size and spacing of the bridges.
7. Click OK.

 Once you create the toolpath, the contour will become part of the toolpath group.

Bridges

Bridges are lifts in a routing offset toolpath that create a tab that maintains the connection between a part that is being cut out and the material from which it is being cut. This tab helps increase the stability of the part so that it doesn’t move as it is being cut. The tabs can then be trimmed away from the part. EnRoute provides several different types of bridges so that you can decide which bridge shape works best for the material type and thickness you are cutting.
After choosing the With Bridges option in routing offset parameters dialog, you have several parameters to define for the bridges, including length, height, type and number. The following table describes the bridge parameters.

Page 156 Working with Toolpaths

Type

This provides the option to select the shape of the bridge. You will probably find a shape that works best with the material you cut. The smooth shapes have the advantage of allowing the machine to move smoothly through the bridge.

Length

This is the length of the bridge. Shorter bridges will work in strong material. If you are cutting soft material, you may need to increase the length of the bridge.

Height

This also lets you adjust the bridge size to fit the material.

By Number

This option lets you choose the number of bridges in the offset.

By Distance

This option lets you choose the spacing of the bridges.

Manual

Rather than specifying the number or spacing of the bridges, you may want to define the specific location of the bridges. Remember though, that even if you specify the bridges by number or distance, you can easily edit the location of the bridges after they are created.


This shows the different types of bridges that are available in EnRoute.

Lift

Ramp

Smooth

Working with Toolpaths Page 157

Ramp Mesa

Smooth Mesa

Deleting Cuts

To delete an unwanted cut from the list of cuts for the strategy, select the cut and click Delete tool.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Editing Cut Parameters

The Cut Parameters dialog allows you to fine-tune the cuts that make up each strategy by changing the cutting parameters from the default values.
For example, if you are cutting a hard material such as aluminum, it likely will be necessary to define a greater number of passes that will use a much smaller portion of the available cutting depth of the tool on each pass
To edit the parameters for a cut:
1. Select the cut in the cut list and click on the ellipses in the Edit column.

Page 158 Working with Toolpaths

2. Edit the cut parameters.
3. Click OK.
The following figure shows the Cut Parameters dialog for the roughing tool in the Routing Offset strategy.

The cut parameters are organized into an explorer list. Click on  or  to expand or collapse an entry in the list.
To the left of the opened/closed symbol is an indicator about the readiness of the parameter values in that category. A green check mark indicates that the values are all ‘legal’. A yellow symbol with a green indicates that the values may not be entirely complete, but that this won’t stop the strategy from being created successfully. A red symbol with an indicates that one or more of the values in that category make it impossible to successfully create the strategy. When the red symbol is displayed, the OK button in the dialog box is also disabled.

Cut Parameter Definitions

Current

Tool

To change the tool that is defined for this cut, select the new tool from the Current

Tool list.

Cut Type

The cut type determines how the toolpath will be created relative to the geometry of the contour. EnRoute will automatically determine the cut type based on the strategy type and the order of cuts applied in the strategy. Any available options are presented so that the user may choose the desired cut type for the selected tool.

In routing offsets, the first cut defined is automatically defined as the Rough cut.

Working with Toolpaths Page 159

This may typically be to the only tool defined in the strategy. If a second cut is defined, it is designated as a Clean cut, and its defined width has the effect of moving the Rough cut away from the geometry by the defined amount. The Clean

cut type allows the Rough cut to remove material around the perimeter of the finished part, to be followed by the Clean cut which finishes the final cutout of the part.

It is now possible to also include a Fine cut on routing offsets. The Fine tool has always been available with Island and Hatch fills, and it now serves a similar purpose with routing offsets. The Fine tool is intended to be able to fit into corners and tight areas in the design into which the rough tool or the clean tool can’t fit.

The following graphic illustrates the letter ‘a’ being cut with three different strategies. The first only uses a Rough cut; the second uses both Rough and Clean cuts; and, the third employs the same Rough and Clean cuts and also adds a Fine cut to ensure that all parts of the geometry can be reached.

There are lots of ways to utilize different cut types, along with different cut depths in order to accomplish complex cutting tasks in EnRoute.

Depths

Surface

Depth

This is the distance from the top of the plate to the top of the cut. A large portion of the time this will be left at the default value of 0.00. There are times, however, when it may be appropriate for the Surface to be set down from the top of the plate, possibly if this cut is to be performed after another cut that has removed part of the material depth.

Final

Depth

This is the depth of the cut, measured from the Surface depth. If the Surface depth is set to 0.00 then the Final Depth is measured from the top of the plate. If the Surface depth is greater than 0.00 then the Final Depth will be measured starting from the Surface Depth. For example, a Surface Depth of 0.50 and a Final Depth of 0.50 would produce an actual cut

depth of 1.00.


Page 160 Working with Toolpaths

Passes

Number This shows the number of passes that will be created. EnRoute calculates the minimum number of passes required based on the Final Depth and

the Max per Pass that is allowed for the selected tool. It is not possible to define a number of passes less than the minimum, but it is quite common to define the number of passes greater than the minimum in order to reduce the amount of material that is removed with each pass.

Widths

Max Per Pass

Actual Per Pass

Final

Pass

Final Pass Depth

Width of Cut

This value is initially calculated based on the dimensions of the selected tool. However, it is possible to reduce this value in order to control the depth of each pass.
This value is calculated based on the number of passes and the Final Cut depth. If a Final Pass is defined, the amount of the final pass is removed from the calculation of the Actual Per Pass value.
If the number of passes is greater than 1, it is possible to designate a Final Pass that will have a cut depth that is different from the other passes. A common use for this is to cut mostly through the material with the passes preceding the Final Pass, and reserve a small thickness that will be cut with the final pass to separate the pieces being cut from the substrate.
This is the depth of the Final Pass. It will obviously be a depth that is less than the Final Depth of the entire cut.
In addition to the cut depth, it is also possible to define a Width of Cut. This is most commonly defined with a Clean Cut, but it may be defined for either a Clean or Rough-cut. If a Clean cut is defined with a 0.00 width, it will essentially be located at the same offset from the contour as the Rough cut. It would ‘clean’ by making another pass next to the rough pass to provide a smoother edge, or to possibly fit into areas that the
rough tool could not. If a width of cut is defined for the Clean cut, then the
Rough cut is offset away from the finished surface by the amount of the width. The Rough cut would leave that width of material that would then
be removed by the Clean cut. The following toolpath images illustrate this

concept.

Number of Steps

This is similar to the concept of Passes with cut depth, except it is the diameter of the tool that controls the Number of Steps that is required for a given Width of Cut. The Number of Steps is calculated automatically based on the Max Step value, and the Width of Cut.

Working with Toolpaths Page 161

Max Step This is the maximum width of material that can be removed in one step.

It is based on the diameter of the tool being used. The software automatically calculates this value to be 90 percent of the tool diameter.
The value can be adjusted so that it is smaller than this, but this is the largest it is allowed to be.

Actual

Step

The Actual Step is calculated based on the Number of Steps and the
Width of Cut values.

Feeds and

Speeds

Shoulder This is an option that provides a way to create a step around the perimeter of the design. The purpose of this option is to allow users to create a ‘lip’ around the edge of the design that is most commonly used with the Inlay option with Routing Offsets and Fills.

Any Clean Pass may be designated as a Shoulder, but it must have a Width of Cut that is larger than 0.00 in order to be designated as a Shoulder. When the Shoulder option is selected, all Clean Pass cuts below it in the list will be positioned out from the Shoulder pass.
This section of the Cut Parameters allows you to specify the feed rates that will be used with this cut. If the tool you are using has feed rates saved for the material you are using, these values will initially reflect the saved values. The units used in the feed rates are initially set to match the values for speed in Preferences Unit section. However, you can change the units to be different if there is a need.

 If your plate has a material selected, the feed rates for that material become the default feed rates for new cuts. If the tool in your cut has feed rates assigned for your material, these feed rates override the material’s feed rates. If no material has been assigned, then the initial feed rates are 0.00.

Feed

Rate

Final Pass Feed

Plunge

Rate

This is the speed that the tool will move in the material when it is cutting.
If the cut is using the Final Pass option, this value represents the speed for this pass.
This is the speed that the tool will move down into the material.

Dwell After plunging into the material, a dwell value will cause the cutting tool to pause for this length of time before feeding into the material.

Direction

Spindle

Speed

This is the speed that the spindle will turn while it is cutting.

 

Conventional

This direction will move the tool ‘with’ the direction that the tool is turning. For a standard exterior cut on a contour, this would be in a counter-clockwise direction.

 

Climb

This is the opposite of conventional. The tool will move ‘against’ the direction that the tool is turning. For an exterior cut, this is in a clockwise direction.

Page 162 Working with Toolpaths

Entry/Exit

Parameters

When a tool begins and ends its cut, it is sometimes desirable to have it move into and out of the cut away from the actual finished edge. The entry and exit provide the means to do this. Each of these may be specified separately; you can have an entry that is an arc, and an exit that is a line.
It is also possible to specify either an arc or line as being ‘3D’. With an entry, this means that the tool will start at the surface depth and progress down to the cut depth over the length of the entry. The exit does the same thing only in reverse. It starts at the end of the cut and progresses up to the surface over its length. With an arc, the arc becomes a helical arc if it is set to 3D.

 If you specify an entry and/or exit as a line, and then enter an angle of 0.0 degrees, the entry/exit will follow the toolpath, even if the toolpath turns over the length of the entry/exit. This can be useful if toolpaths are close together and you want to make sure they don’t interfere.


The diagram below depicts how the dimensions of the entry and exit are specified.

Radius

Angle

Length

Angle

3D Toolpaths

This option designates whether this cut will be a 3D pass or not. A 3D toolpath may be created using a conic, engraving or tapered tool. The difference is that it uses the beveled shape of the tool to create a beveled edge. It also will move up into corners to get as far into the corners as the tip dimension of the tool will allow.
As you can imagine, a 3D Toolpath designation is only appropriate in certain situations, and with certain tools. The software monitors the type of cut and the type of tool that has been specified, and then controls when the 3D Toolpaths option may be selected. Also, this option is not available at all licensing levels of the software. If your version does not have the 3D Toolpaths option enabled, it is possible to enable this function by upgrading the software license.
The 3D option is a very powerful option, allowing a very different type of cut from any of the toolpaths that are strictly 2D. 3D toolpaths may be created for cleaning cuts with Routing Offsets, Island Fills, and Hatch Fills. With the Engrave Strategy, the 3D toolpath will likely serve as the primary option on many jobs.
The following figure provides an illustration of some of the 3D toolpaths that may be created.

Working with Toolpaths Page 163

Saving Cut Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Cut Settings from a Template

To load the settings previously saved as a template, select the template from the Cut list.

 It is possible to load a cut template that was defined for one Strategy type into the Cut Parameters dialog for a different strategy type. Since different strategies use different cut parameters, it is possible that not all of the parameters for the new cut will be defined in the template.

Creating Open Contour Offset Toolpaths

Menu: Toolpath / Offset Open Contours

Toolbar: Toolpath / Routing Offset/ Router Offset Open Contour

The Open Contour Offset is closely related to the Routing Offset strategy described in the previous sections. The key difference is that the Routing Offset strategy is designed to be used with closed contours, and Open Contour Offset is designed for open contours.

 You will notice that it is not possible to define bridges with an open contour strategy. It is possible, however, to add bridges to open contours offsets by manually inserting them using the Edit Bridges tool available in the Toolpath menu. Bridges on open contour offsets may be inserted and edited the same as other bridges, using this tool.

Page 164 Working with Toolpaths

To create a toolpath using the Open Contour Offset strategy:
1. Select the contour you want the toolpath to follow.
2. Click and hold Routing Offset  then Offset Open Contour
3. In the Open Contour Offset dialog, select the desired tool from the Available Tools list and click Add Tool.
 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

 The first tool in the list is always defined as the Rough tool, and it is typically used as the main cutting tool. Any additional tools serve as Clean tools, primarily used as a final pass to clean up cutting marks from the Rough tool, or to fit into areas that the Rough tool couldn’t.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.
6. Set the Open Contour Offset parameters:

Side Rather than defining whether the offset is to be internal or external as with the Routing Offset, it is necessary to define which side of the contour to place the toolpath. Left and Right are determined as if you are facing in the direction of the contour. If it is located in the middle, the toolpath is placed on top of the open contour.

Left   Middle   Right  

Working with Toolpaths Page 165

With

Relief

One of the common uses of an Open Contour Offset is to cut out sections around the perimeter of a design. For example, you might use a standard routing offset to cut out a simple rectangle, and then use an Open Contour Offset to cut out additional shapes around the outside of the rectangle. In certain materials, and especially wood, it is necessary for the tool to move into the material rather than moving from inside the material out in order to minimize the risk of the material

‘blowing out’ as the tool leaves the material.

The With Relief option allows you to define a segment of the toolpath at its end to move in rather than out so that you can ensure that the toolpath won’t move the tool out of the material as it is cutting.

The graphic below illustrates an open contour that uses Relief at the end. The left end of the toolpath is the ‘end’ with Relief. Notice the direction arrow pointing the other way: this is part of the Relief section.

If the With Relief option is selected, the following additional parameters are displayed.

 

Relief

Length

This is the length of the section at the end of the toolpath that will move back in from the end.

 

Relief

Overlap

It is possible to overlap the two sections to ensure a clean cut.

 

Cut End

First

If this is selected, the Relief section of the toolpaths will be cut before the rest of the Open Contour Offset toolpaths.

7. Click OK.

 Once you create the toolpath, the contour will become part of the toolpath group.

Deleting Cuts

To delete an unwanted cut from the list of cuts for the strategy, select the cut and click Delete tool.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Page 166 Working with Toolpaths

Editing Cut Parameters

The process for editing cut parameters for the Open Contour Offset strategy is nearly identical to that
for the Routing Offset strategy (see “Editing Cut Parameters”).
The two exceptions to this are:
 It is not possible to define the toolpaths as 3D toolpaths so the 3D Toolpath option is not available.
 The direction of the toolpath is defined by the direction of the contour, so the Direction cut parameter is not available.

 Note that you are able to define widths for each type of cut. This allows you to use open contours to cut out areas that are wider than the tool you are using to perform the cut.

Kerf Compensation Toolpaths

The Kerf Compensation toolpath was designed primarily to work with CNC cutting devices other than routers. It is essentially the same as a routing offset. The dialog was designed to be simpler, and to offer only the necessary parameters for 2D cutting, without such things as bridges, or multiple tool options. In addition, kerf compensation provides the option of adding toolpath loops in and out of external corners. The size of the loops can also be defined. With plasma and water jet cutting, it is important that the cutting head maintains as much of a uniform cutting speed. Loops allow the cutting to maintain a constant speed into and out of the corner, helping to provide a more uniform cut.

Menu: Toolpath / Kerf Compensation

Toolbar: Toolpath / Kerf Compensation


Working with Toolpaths Page 167

Parameter

Value

Kerf Width

.05, .10, or .15 are present by default. Additional kerf width choices may be added.

External (male)

If checked, the toolpaths will follow the outside of the contour.

Internal (female)

If checked, the toolpaths will follow the inside of the contour.

Feed Rate

This is the speed that the tool will move in the material when it is cutting.

Weld Offsets

If checked, overlapping offsets will be welded together to form a single toolpath group. If cleared, overlapping offsets will be left the way they are.

Loop Corners

This option allows the toolpath to be created with loops on external corners. The loops allow the tool to go around the corner without having to decelerate around the corner. With plasma cutting, this can provide for a more uniform cut, and cleaner corners.

Sharp Corners

If this option is checked, the toolpath offsets form square corners.

Direction Conventional

For a standard exterior cut on a contour, this would be in a counter-clockwise direction.

Climb

For an exterior cut, this is in a clockwise direction.

Entry/Exit Parameters

When a tool begins and ends its cut, it is sometimes desirable to have it move into and out of the cut away from the actual finished edge. The entry and exit provide the means to do this.

Entry Type

Choose the type of Entry and enter the parameters.

Exit Type

Choose the type of Exit and enter the required parameters.

Daisy Chain Toolpaths

Menu: Toolpath / Daisy Chain

Toolbar: Toolpath / Daisy Chain

Router users now have the option to Daisy Chain the toolpaths. Daisy Chain toolpaths can in some applications improve efficiency by allowing the cutting to be done without having to lift the tool out of the material as often.

Page 168 Working with Toolpaths

Example:
1. Apply a Routing Offset toolpath. Be sure that an Entry and an Exist have been defined with the Routing Offset.
2. Select the objects with the Routing Offset toolpath.
3. Click on the Daisy Chain Icon This will create the Daisy Chain Toolpath which connects the toolpaths together so the tool does not lift more than necessary.
In looking at these before and after images of the toolpaths, you will notice that the Daisy Chain process has connected the individual toolpaths from the separate objects. It has also moved the start points, as necessary to minimize the movement of the tool within the material. During the Daisy Chain process, it may still be necessary for the tool to lift out of the material in order to reach parts that can’t be reached otherwise, or to maintain a reasonable distance between parts and within the material.
This method was created primarily for use with Plasma cutting machines. With these machines the cutting tip on the torch is a consumable part that is used up more quickly when the cutting torch is started and stopped for each part. For these tools it is often more cost effective for the cutting to continue between parts.

Hatch Fill

Menu: Toolpath / Hatch Fill

Toolbar: Toolpath / Hatch Fill

 The Hatch Fill strategy can only be used with closed contours.

The Hatch Fill Strategy is used to create toolpaths to mill a surface down to a defined depth using toolpaths that move back and forth across the area to be milled. This option is used most often to mill out larger areas of material that typically don’t have a lot of thin sections, but it can be used on any artwork.

Working with Toolpaths Page 169

Types of Cuts

There are three types of cuts that can be defined in the Hatch Fill Strategy, the Fill Cut, Fine Cut, and
Clean Cut. Each of these is explained below.

Fill Cut

This is the tool that will perform the Hatch Fill. You will almost exclusively use an end mill tool to perform the fill. In addition to the standard cut parameters that have been described previously, with the Fill Cut it is necessary to define two additional key parameters – Overlap and Angle. See “Editing Cut Parameters” for details.

Fine Cut

The Fine Cut is optional. If it is used, a tool that is smaller in diameter than the Fill tool is selected to fit into sections of the design that the fill tool was not able to fit into. This will be corners and any other thin areas that are too small for the Fill tool. The Fine Cut uses an Island Fill strategy to fill in areas that require more than one width of the tool. For this reason, it is also necessary with the Fine Cut to specify the amount of overlap between adjacent toolpaths.
The following screen shot shows a Hatch fill with a Fine Cut used to fit into the areas where the fill tool
won’t fit.

Clean Cut

The final toolpath option with the Hatch fill is the Clean Cut. This defines a tool that creates toolpaths that are offset from the contours. The Clean Cut is used to improve the edge quality of the finished cut, or to create a 3D toolpath around the perimeter of the design.
The following image shows a Hatch fill that includes a 3D Clean Cut. This combination of using a fill pattern along with a 3D clean cut is a very common technique used in many engraving, woodworking and sign-making applications. Many times there is a need to utilize a 3D engraving toolpath, but the material doesn’t permit the 3D toolpath to go to the ‘bottom’ of the design. In this case, the fill can be used to define the bottom of the design.

Page 170 Working with Toolpaths


To create a toolpath using the Hatch Fill strategy:
1. Select the contour you want the toolpath to follow.
2. Click Hatch Fill
3. In the Hatch Fill dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

 The first tool in the list is always defined as the Rough tool, and it is typically used as the main cutting tool. Any additional tools serve as Clean tools, primarily used as a final pass to clean up cutting marks from the Rough tool, or to fit into areas that the Rough tool couldn’t.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.
6. Set the Hatch Fill parameters:

Inlay This defines whether this strategy is part of an inlay project. If this fill will be used as the female part of an inlay project, it is necessary for the software to modify the toolpaths to compensate for the dimensions of the tool. Also, you will need to define the inlay gap, which is the spacing between the male and female portions of the inlay. A gap is needed to allow the two parts of the inlay to fit together. The screen image below shows two contours that have been hatch filled. The contour on the right has also been defined as an inlay to illustrate how the toolpaths are modified at the corners.

Working with Toolpaths Page 171



Without Inlay With Inlay

Optimization There are three different options regarding the way in which the hatch toolpaths are ordered within the contour. In the machining industry there are many different viewpoints regarding how ‘pocket milling’ toolpaths should be ordered in order to be most efficient. The software utilizes a method that is intended to minimize tool lifts in the fill, but not necessarily to prevent tool lifts.

In many cases it is not practical to attempt to eliminate tool lifts without breaking other rules that the software enforces. The software does not allow any of the hatch toolpaths to pass over any part of the hatch area more than one time. Also, it strictly enforces a back-and-forth pattern over the entire hatch area. We feel that this results in a more aesthetically pleasing finish on the hatch surface, and it is consistent with methods employed by other machining packages.
A second important option for ordering hatch toolpaths is to make them compatible with a specific type of engraving tool that utilizes a ‘Nose Cone’ that maintains a constant depth of cut for the tool. This requires that the hatch toolpaths progress from one side of the fill to the other, always maintaining an edge of uncut material next to the nose cone.
Finally, the software provides the option of having the cleaning pass that is associated with the hatch toolpath be cut before the hatch toolpaths. This can be a desirable option when cutting certain types of material, such as certain woods.
7. Click OK.

 Once you create the toolpath, the contour will become part of the toolpath group.

Deleting Cuts

To delete an unwanted cut from the list of cuts for the strategy, select the cut and click Delete tool.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Page 172 Working with Toolpaths

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Editing Cut Parameters

The process for editing cut parameters for the Hatch Fill strategy is nearly identical to that for the
Routing Offset strategy.
The one key difference lies in the parameters for the Fill cut, where two additional parameters are defined under Fill:

 Overlap – This parameter defines how much adjacent toolpaths will overlap each other in the fill.

The default value that is created when the Fill Cut is created is 50 percent. Legal values are 0 to
99 percent. When cutting soft materials, you may typically reduce the overlap 10 or 20 percent. However, when cutting denser materials, it may be desirable to increase the overlap percentage
to 70 percent or more. You will also notice that the overlap percentage has an effect on the finished surface pattern, so you may at times use the overlap to create a desired effect.

 Hatch Angle – This angle determines the angle (measured from horizontal) that will be used to create the Hatch Fill. Most of the time you will likely use either 0-degrees for horizontal or 90- degrees for vertical toolpaths. Other angles can be used to create an effect, or to better utilize the shape of the area to be milled.

Creating Island Fill Toolpaths

Menu: Toolpath / Island Fill

Toolbar: Toolpath / Island Fill

The Island Fill strategy can only be used with closed contours.
The Island Fill Strategy is very similar to the Hatch Fill Strategy. The way that the two are defined is virtually identical. The results, however, are quite different because of the pattern of the fill toolpaths that are created.

Working with Toolpaths Page 173



Hatch Fill Island Fill

Island Fill vs. Hatch Fill

There are two main factors to be considered when choosing a fill strategy. First, select the strategy that will most efficiently mill the area to be milled. Typically, if you have a large open area, a Hatch Fill will be most efficient. On the other hand, if you have a design that is made up of long, thin sections, an Island Fill will most likely work best.
The second reason for choosing one method over the other is based on whether the tooling pattern that will be left in the milled area is important. As you work with these strategies, you will see that each of them will create a different pattern, and there may be times when this pattern is important in deciding which strategy is appropriate.
The best thing is to experiment with each and then decide for yourself which method works best in any given situation.

Creating an Island Fill

To create a toolpath using the Island Fill strategy:
1. Select the contour you want the toolpath to follow.
2. Click Island Fill
3. In the Island Fill dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

 The first tool in the list is always defined as the Rough tool, and it is typically used as the main cutting tool. Any additional tools serve as Clean tools, primarily used as a final pass to clean up cutting marks from the Rough tool, or to fit into areas that the Rough tool couldn’t.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.
6. Set the Island Fill parameters:

Page 174 Working with Toolpaths

Inlay This defines whether this strategy is part of an inlay project. If this fill will be used as the female part of an inlay project, it is necessary for the software to modify the toolpaths to compensate for the dimensions of the tool. Also, you will need to define the inlay gap, which is the spacing between the male and female portions of the inlay. A gap is needed to allow the two parts of the inlay to fit together. The screen image below shows two contours that have been hatch filled. The contour on the right has also been defined as an inlay to illustrate how the toolpaths are modified at the corners.



Without Inlay With Inlay

Optimization There are three different ways in which the fill toolpaths can be ordered within the contour. In the machining industry there are many different viewpoints regarding how ‘pocket milling’ toolpaths should be ordered in order to be most efficient. The software utilizes a method that is intended to minimize tool lifts

in the fill, but not necessarily to prevent tool lifts.
In many cases it is not practical to attempt to eliminate tool lifts without breaking other rules that the software enforces. The software does not allow any of the hatch toolpaths to pass over any part of the hatch area more than one time. Also, it strictly enforces a uniform pattern over the entire hatch area. We feel that this results in a more aesthetically pleasing finish on the hatch surface, and it is consistent with methods employed by other machining packages.
A second important option for ordering hatch toolpaths is to make them compatible with a specific type of engraving tool that utilizes a ‘Nose Cone’ that maintains a constant depth of cut for the tool. This requires that the hatch toolpaths progress from one side of the fill to the other, always maintaining an edge of uncut material next to the nose cone.
Finally, the software provides the option of having the cleaning pass that is associated with the hatch toolpath be cut before the hatch toolpaths. This can be a desirable option when cutting certain types of material, such as certain woods.
7. Click OK.

 Once you create the toolpath, the contour will become part of the toolpath group.

Deleting Cuts

To delete an unwanted cut from the list of cuts for the strategy, select the cut and click Delete tool.

Working with Toolpaths Page 175

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Editing Cut Parameters

The process for editing cut parameters for the Hatch Fill strategy is nearly identical to that for the
Routing Offset strategy (see “Editing Cut Parameters”).
One of the options available in the cut parameters for the fill tool in the Island Fill strategy is whether to use Corner Tags. Corner tags are used to ensure that the specified overlap value is enforced throughout the fill. This can be very important when you use an overlap of less than 50 percent, because it ensures that the entire fill area gets milled. The following graphic illustrates a fill toolpath with and without corner tags.


With corner tags Without corner tags

Spiral Fill Toolpaths

Menu: Toolpath / Spiral Fill

Toolbar: Toolpath / Hatch Fill / Spiral Fill

The Spiral Fill strategy is essentially the same as the Island fill, except that it creates a spiral pattern for filling the selected contours. This can be very useful for certain design elements, but it is typically only useful for objects that are round or near round. On round contours it allows the toolpath to be created as a single toolpath. This eliminates the need for the tool to step in after every trip around. The advantage is that this is more efficient, and it can also improve the aesthetics of the tooling marks that are left on the milled surface.
On objects that are not round, the toolpath must stop where it intersects the edge of the part, which

Page 176 Working with Toolpaths

requires the tool to lift up and then move to the next portion of the toolpath. This could require many more tool lifts than would be necessary using either a standard Hatch or Island fill.


Working with Toolpaths Page 177

Drill Tools Menu: Toolpath / Drill Toolbar: Toolpath / Drill

Drill points are similar to toolpaths, but they are not the same. Many CNC machines are able to respond differently to drill commands than they do to standard toolpath commands. For this reason, the software creates drills as a different type of object so that when this information is sent to the machine, the driver is capable of determining how much drill information a specific machine requires, and how much should be controlled by the machine. For the most part you don’t have to think about drills at this level, but it is important to know that they differ from toolpaths.

There are six different strategies used to create drill points. Each of these strategies is identical in the way that they create the drill points, and in how Drill Cut Parameters are defined. They differ in how they arrange the drill points.

Creating Drill Points

Menu: Toolpath / Drill / Drill Point

Toolbar: Toolpath / Drill / Drill Point

The Drill Point strategy creates a single drill point at the location specified. To create a drill point:
1. Click Drill then Drill point
2. In the Drill Point dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
3. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill hole.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
4. Enter the Drill Point parameters:

Page 178 Working with Toolpaths

X Coordinate and Y Coordinate

These are the X and Y coordinates for the drill point.

By Graphic

If this box is checked, the X and Y coordinates will be selected with the mouse.

5. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
6. Click OK.
7. If you checked the By Graphic box, click with the mouse to place drill points on your design.
Right-click to release the tool. If the By Graphic box was cleared, a single drill point will be
created at the specified coordinates.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Creating Drill Circles

Menu: Toolpath / Drill / Drill Circles

Toolbar: Toolpath / Drill / Drill Circles

The Drill Circle strategy creates a circular pattern of drill points, centered at the location specified. To create a drill circle:
1. Click Drill then Drill circle
2. In the Drill Point dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
3. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill holes.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
4. Enter the Drill Circle parameters:

Working with Toolpaths Page 179

Circle Diameter

This is the diameter of the circle around which the drill points will be placed. This dimension must be greater than zero to be legal.

Angle

You may want to rotate the drill points on the circle to place them correctly. When the angle is zero the first drill point will be placed on the circle directly to the right of center. You may enter a value between 0 and 360 for this value.

Number of Holes

This specifies the number of drills to be placed. A value of 1 or greater should be entered.

X Coordinate and

Y Coordinate

These are the X and Y coordinates for the center of the circle of drill points you are defining.

By Graphic

If this box is checked, the X and Y coordinates will be selected with the mouse.

5. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
6. Click OK.
7. If you checked the By Graphic box, click with the mouse to place drill circles on your design.
Right-click to release the tool. If the By Graphic box was cleared, a single drill circle will be created at the specified coordinates.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Creating Drill Arrays

Menu: Toolpath / Drill / Drill Array

Toolbar: Toolpath / Drill / Drill Array

The Drill Array strategy creates a ‘matrix’ of drill points with a set number of rows and columns, and a
specified amount of spacing between them.
3. Click Drill then Drill Array
4. In the Drill Array dialog, select the desired tool from the Available Tools list and click Add
Tool.
 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

Page 180 Working with Toolpaths

5. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill holes.

 It is possible to enter fractional values such as ½ in order to let the program calculate the decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of

3/16 is 0.1875.
6. Enter the Drill Array parameters:

Columns

The number of vertical drill columns.

Rows

The number of horizontal drill rows.

Spacing

The options that define the spacing of the drill points in the array.

 All spacing is applied between the center drill points of the columns and rows, not between the outside edges of the drill cuts.

 

Width by overall width

If selected, enter the overall width of the array. The drill points will be evenly spaced horizontally within this width.

 

Width by horizontal spacing

If selected, enter the amount of horizontal space between the columns of drill points.

 

Height by overall height

If selected, enter the overall height of the array. The drill points will be evenly spaced vertically within this height.

 

Height by vertical spacing

If selected, enter the amount of vertical space between the rows of drill points.

X Coordinate and Y Coordinate

These are the X and Y coordinates for the center of the array of drill points you are defining.

By Graphic

If this box is checked, the X and Y coordinates will be selected with the mouse.

7. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
8. Click OK.
9. If you checked the By Graphic box, click with the mouse to place drill arrays on your design.
Right-click to release the tool. If the By Graphic box was cleared, a single drill circle will be created at the specified coordinates.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Working with Toolpaths Page 181

Creating Drill Points in the Centers of Contours

Menu: Toolpath / Drill / Drill Points in Center

Toolbar: Toolpath / Drill / Drill Points in Center

 The Drill Centers strategy can only be used with closed contours.
The Drill Centers strategy creates drill points at the centers of each of the selected contours. You can specify to select only circles and a range of sizes to use, if desired.
1. Select the contours you want to create drill points in the center of.
2. Click Drill then Drill centers
3. In the Drill Centers dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill hole.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Select the Drill Centers parameters:

All contours

If selected, holes will be drilled in the centers of all the selected contours.

Circles only

If selected, holes will only be drilled in the centers of the selected circles. Selecting this option displays the following additional options.

 

All circles

If selected, holes will be drilled in the centers of all selected circles.

 

By diameter

If selected, holes will be drilled in the centers of all selected circles whose diameters are within the Tolerance of the Check Diameter specified.

6. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
7. Click OK.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Page 182 Working with Toolpaths

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Creating Drill Points Along a Contour

Menu: Toolpath / Drill / Drill Contour

Toolbar: Toolpath / Drill / Drill Contour

The Drill Contours strategy creates drill points along selected contours, based on the number and spacing specified.
1. Select the contours you want to create drill points in the center of.
2. Click Drill then Drill contours
3. In the Drill Contours dialog, select the desired tool from the Available Tools list and click

Add Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill hole.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Select the Drill Contours parameters:

Spacing

Type

Select the way the drill points will be placed along the contours you have selected:

 

Hold

Number

A specified number of drill points will be spaced evenly along the length of the contours. The number is specified by the Number of Holes parameter.

 

Hold

Spacing

Drill points will be spaced along the length of the contours at a distance specified by the Spacing parameter.

 

Corners

Drill points will be created at all corners in the contours.

 Circles and ellipses have no corners, and will have no drill points created for them.

 

Inside

Corners

Drill points will be created at all inside corners in the contours.

 Circles and ellipses have no corners, and will have no drill points created for them.

 

Outside

Corners

Drill points will be created at all outside corners in the contours.

 Circles and ellipses have no corners, and will have no drill points created for them.

Working with Toolpaths Page 183

Number of Holes

The number of holes used with the Hold Number spacing type.

Spacing

The spacing between drill points used with the Hold Spacing type.

6. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
7. Click OK.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Creating Drill Points at the Corners of the Plate

Menu: Toolpath / Drill / Drill Corners

Toolbar: Toolpath / Drill / Drill Corners

 The Drill Corners strategy is available only if a plate has been defined.
The Drill Corners strategy creates drill points in the corners of the plate, with the ability for additional drills in between each corner.
1. Click Drill then Drill Corners
2. In the Drill Corners dialog, select the desired tool from the Available Tools list and click Add

Tool.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
3. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill hole.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
4. Enter the Drill Corners parameters:

Inset X

The horizontal inset from the corners of the plate. If it is left at 0.00 the drill points will be centered on the corners of the plate.

Inset Y

The vertical inset from the corners of the plate.

Page 184 Working with Toolpaths

Add Copies X

Enter a number here to create additional drill points spaced evenly between the corner drills in the horizontal axis.

Add Copies Y

Enter a number here to create additional drill points spaced evenly between the corner drills in the vertical axis.

5. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
6. Click OK.
7. If you checked the By Graphic box, click with the mouse to place drill points on your design.
Right-click to release the tool. If the By Graphic box was cleared, a single drill point will be
created at the specified coordinates.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Editing Drill Cut Parameters

The drill cut parameters are very similar to the cut parameters in the other strategies, with a couple of key differences. They are all the same within the different Drill Strategies. The following sections identify the unique cut parameters for the drill.

Diameter by tool vs. Exact diameter – If the ‘Diameter by tool’ option is selected, the drill will truly be a drill point, meaning that the size of the hole is based entirely on the diameter of the tool at a given depth.

If the ‘Exact diameter’ option is selected, the user can define a diameter that is larger than the tool’s diameter, and the drill point will be created as a circle. The circle will be sized to make the drill hole the diameter specified for the selected tool at the depth defined.
It is important to point out that EnRoute takes into account the shape of the tool in determining the diameter of the tool at a given depth. If you are using a conic tool to create the drill, and specify an exact dimension at a depth that is less than the height of the bevel, EnRoute will automatically take into account the real diameter of the tool at the depth specified.
The following screen image illustrates a number of drills that show drills defined both ‘by tool’ and ‘by diameter’.

Working with Toolpaths Page 185


Countersink – If a tool is selected that is capable of engraving (conic, engrave, tapered) then if the ‘Diameter by tool’ option is selected, another option is made available. Countersink lets you specify the diameter of a hole you would like to make that takes into account the bevel on the tool. EnRoute will then automatically calculate how deep the tool should go in order to create a countersink hole with an outer diameter as specified. This is an option designed to aid in designing drill holes that will accommodate screws of a certain size in the finished piece.

Depths, Passes, Feeds and Speeds – These parameters are pretty much just the same in the drills as they are in all of the other strategies. Review the detailed descriptions provided in the Routing Offset Strategy section for more information.

Page 186 Working with Toolpaths

Creating Slot Toolpaths

Menu: Toolpath / Slots

Toolbar: Toolpath / Slots

A slot is a special tool that allows you to define a tool to cut along a line, making a slot that is the width of the tool diameter. Like drills, slots can include more than one tool, and more than one depth.
1. Click Slots
2. In the Slot dialog, select the desired tool from the Available Tools list and click Add Tool.
 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.
3. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the drill hole.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
4. Enter the Drill Corners parameters:

Start X and Y Coordinates

The X and Y coordinates of the starting point of the slot.

End X and Y Coordinates

The X and Y coordinates of the endpoint of the slot. These must be different than the coordinates of the starting point.

By graphic

If this box is checked, the coordinates of the starting and end points will be selected with the mouse.

Back and forth

If checked, the tool will move from the start point to the end point and return to the starting point before being lifted from the plate.

5. Add additional drill cuts using other tools as necessary. All cuts will share the same drill point coordinates.
6. Click OK.
7. If you checked the By Graphic box, click with the mouse to place the starting and end points on your design. Right-click to release the tool. If the By Graphic box was cleared, the slot will be created between the specified coordinates.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Working with Toolpaths Page 187

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Creating an Engrave Toolpath

Menu: Toolpath / Engrave

Toolbar: Toolpath / Engrave

Engraving is a traditional machining function that has many applications. In one sense it is the most straightforward type of toolpath creation, and in another sense it is the most complex.
Two-dimensional engraving is essentially just the creation of toolpaths that follow the contours of the contours at a specified depth. 3D toolpaths offer better results: they are able to cut out sharp corners better when using conic tools, for instance. However, 3D toolpaths using conic tools require a tremendous number of computations in order to accurately and reliably create the desired effect.
For the user it is a simple matter of deciding if the toolpaths should be 2D or 3D. The software then performs the required computations to create the appropriate type of toolpaths.

 If you are defining a deep engrave strategy it is often better to use a fill strategy with a 3D Clean pass so that if the engrave toolpath doesn’t go all the way to the bottom, the fill tool can finish milling the bottom surface.

1. Select the contour you want the toolpath to follow.
2. Click Engrave
3. In the Engrave dialog, select the desired tool from the Available Tools list. Click Add Tool.
 The Sort tools by list determines the parameter that is used to sort the Available Tools list.
It can also filter the tools that are displayed so that only a certain type of tool is visible.

 Only those tools that are capable of engraving, including conic, engrave and tapered tools, may be defined as engrave cuts.

 The first tool in the list is always defined as the Engrave tool, and it is typically used as the main cutting tool. Any additional tools serve as Rough tools, primarily used to remove excess material. The typical scenario in the case of a deep engraving toolpath is to define a Rough cut that uses an end mill tool.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.
6. Set the Engrave parameters:

Page 188 Working with Toolpaths

3D Engrave toolpath

Check to create the engrave cut as a 3D engrave toolpath. If cleared, the cut will be a 2D toolpath.

 Remember that only tools capable of 3D engraving, including conic, engrave and tapered tools, may be defined as 3D engrave toolpaths.

External or

Internal

If the 3D option is selected for the engrave toolpath, it is necessary to define whether the toolpaths should pass to the inside or the outside of the contours in the selection. Most typically, the engraving toolpaths will be defined on the inside of the contours. The following images show 3D toolpaths created on the inside and outside of a contour:


Internal External

 Because external 3D toolpaths require all objects in the selection to be combined into one toolpath group, they are not compatible with other types of toolpaths in a contour. If existing toolpath groups are included in the selection, their toolpaths will be deleted when these toolpaths are created.

7. Click OK.

 Once you create the toolpath, the contour will become part of the toolpath group.

Square Corner for External 3D Engrave

With external Engrave toolpaths, an available option is to choose whether or not to use Square

Corners.



Working with Toolpaths Page 189



Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Engrave Cut Parameters

The engrave cut parameters include the standard categories of Depths, Passes, Feeds and Speeds, and Direction. The first cut tool is automatically defined as the Engrave tool, and if a second tool is defined, it is classified as the Rough tool. Toolpaths for the Rough tool are only created if require d by the Engrave cut.

Page 190 Working with Toolpaths

Creating Pyramid Toolpaths

Menu: Toolpath / Pyramid

Toolbar: Toolpath / Pyramid

The Pyramid Strategy allows you to create a beveled type of artwork that is also commonly referred to as chiseled or sculpted artwork. The Pyramid Cut utilizes a beveled tool, most commonly a conic tool, to create the beveled effect. This cut is unique in that it is necessary for the software to calculate the depth of cut based on the selected tool, and the selected contours. The cut depth is based on the widest ‘stroke’ in the design. The software then places toolpaths at the proper depth based on the maximum cut depth it calculates.
The finished result from this strategy can be very striking, and it can be effectively utilized on very small pieces all the way up to designs that are several feet tall and wide.

 Remember to check the Pyramid parameter for ‘Move to bottom of plate’ in order for the Return

Height to be created correctly.
1. Select the contour you want the toolpath to follow.
2. Click Pyramid
3. In the Pyramid dialog, select the desired tool for the pyramid cut from the Available Tools list and click Add Tool.

 Only those tools that are capable of engraving, including conic, engrave and tapered tools may be defined as pyramid cuts.

 The Sort tools by list determines the parameter that is used to sort the Available Tools list. It can also filter the tools that are displayed so that only a certain type of tool is visible.

4. In the tool listing that appears in the list of cuts at the top of the dialog, set the Depth of the cut.

 It is possible to enter fractional values such as ½ in order to let the program calculate the

decimal equivalent. That way it isn’t necessary to remember that the decimal equivalent of
3/16 is 0.1875.
5. Add additional cuts using other tools as necessary.

Working with Toolpaths Page 191

 The first tool in the list is always defined as the Pyramid tool, and it is typically used as the main cutting tool.

 The second tool is defined as the Rough tool, and is primarily used to remove excess material.

The Rough tool is typically a medium-sized end mill tool.

 The third tool is defined as the Offset tool, and is used to cut around the outside of the Pyramid cut, either to create a relief, or to cut the pyramid away from the surrounding plate.

6. Set the Pyramid parameters:

Return

Height


The height of any vertical ‘edge’ that is to be created below the beveled portion of the contour. In order for the return height to be meaningful, it is necessary to move the toolpath down to the bottom of the material so that the return will be created when the pieces are cut out.

Surface Depth

Cut Depth

Plate

Thickness

Return Height

Page 192 Working with Toolpaths

Move to bottom of plate

If checked, the bottom edge of the return height (if any) will be aligned with the bottom of the plate.
If this option is cleared, the toolpaths will be placed such that the top of the bevel will be at the surface of the material.
7. Click OK.

 Once you create the toolpath, the contour will be part of the toolpath group.

Saving Strategy Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Strategy Settings from a Template

To load the settings previously saved as a template, select the template from the Strategy list.

Pyramid Cut Parameters

The cut parameters in this strategy are much the same as the other strategies. The key difference is that for the most part the software will automatically define the depths of the cuts for you based on the selections you make at the strategy level. It is possible to override the Surface Depth for the cuts, although this is not typically recommended.
You may at times want to increase the number of passes for a given cut in order to take into account material densities. By default, EnRoute will utilize 90 percent of the tool’s cutting depth on the Pyramid cut. For soft material this is likely appropriate, but for denser material such as wood, you will likely want to decrease the pass depths by increasing the number of passes.

Editing Toolpaths

Menu: Toolpath / Edit Toolpaths

After toolpaths are created, the software maintains all of the information about how the toolpaths were created. You can edit the toolpaths at any time and change the cuts and parameters that define the toolpath. When you are finished, the software regenerates the toolpath using the new settings.
To edit a toolpath:
1. Select the toolpath.
2. From the Toolpath menu, select Edit toolpaths.

Working with Toolpaths Page 193

3. If the toolpath group contains more than one strategy, you will be prompted to choose which strategy to edit. Select the strategy you want to edit and click OK.

4. In the dialog for the strategy, make the desired changes to the settings and click OK.

Editing the Toolpath Plan

The plan is the set of all strategies contained in a toolpath group. Editing it allows you to edit the individual strategies, delete them, add new strategies, and save the entire plan as a template.

Accessing the Plan

To access the plan:
1. Select the toolpath.
2. From the Toolpath menu, select Edit toolpaths.
3. If necessary, select a strategy and click OK.
4. In the strategy dialog, click Edit Plan.

Editing Strategies

To edit a strategy:
1. Select the strategy in the strategy list and click on the ellipses in the Edit column.
2. Edit the strategy in the strategy dialog.
3. Click OK.

Page 194 Working with Toolpaths

Adding Strategies

To add a strategy to the plan:
1. Click on the appropriate button under Add Strategy.
2. Create the strategy using the strategy dialog.
3. Click OK.

Removing Strategies

To delete a strategy from the plan:
1. Select the strategy in the strategy list.
2. Click Remove.

Clearing All Strategies

To delete all the strategies from the plan, click Clear.

Saving Plan Settings as a Template

To save the current settings as a template:
1. Click the Save as button.
2. Type a name for the template and click OK.

Loading Plan Settings from a Template

To load the settings previously saved as a template, select the template from the Plan list.

Editing Entry/Exit Points

Each cut in a toolpath has its own entry and exit points. These are the points at which the tool will enter and exit the plate material as it makes the cut. Often the entry and exit points are at the same point.
By default, the entry and exit points are drill points, indicating that the tool will drill straight down into the material at the start point and lift straight out at the end point. The entry and exit points may also be arcs or lines, however, in which case the cutting tool will move laterally into the material on the line or arc specified and then begin cutting along the toolpath. If a 3D line or arc is specified, the tool will move down into the material on a diagonal line as viewed from the side.



Working with Toolpaths Page 195

Points Arcs Lines

 Not all toolpath start points may be moved, and not all start points are eligible to include Entry/Exit toolpaths. Generally, this type of editing is most applicable to Routing Offset toolpaths.

Moving Entry/Exit Points

Menu: Toolpath / Edit Entry/Exit

To move an entry/exit point:
1. Select the toolpaths you want to edit.
2. From the Toolpath menu, select Edit Entry/Exit.
3. Click on the entry/exit point and drag it to its new location along the toolpath.

 Moving entry/exit points on a toolpath can use the snap settings to more precisely locate the desired point.

Moving Entry/Exit Points for Individual Cutting Passes

By default, each of the cutting passes for a given cut will have identical entry/exit points. When you move the entry exit points for one, you move them for all of the cutting passes.
To move the entry/exit points for a single cutting pass:
1. Press F10.
2. In the View Setup tab of the Setup Preferences dialog, set Depth to the cutting depth of the pass you want to edit.
3. Click OK.

 Only the single cutting pass at this depth is displayed/editable.

4. Select the toolpath you want to edit.
5. From the Toolpath menu, select Edit Entry/Exit.
6. Click on the entry/exit point and drag it to its new location along the toolpath.
7. Press F10.
8. In the View Setup tab of the Setup Preferences dialog, set Depth back to All depths.
9. Click OK.

Editing Entry/Exit Cut Parameters

Menu: Toolpath / Edit Entry/Exit

In order to change the type of entry/exit point in use, or to make them 3D, it is necessary to edit the entry/exit parameters for a cut.

Page 196 Working with Toolpaths

The entry/exit parameters can be edited along with the other cut parameters for the cut, or they can be edited separately.
For details on editing all cut parameters, see “Editing Cut Parameters”.
To edit only the entry/edit points for a toolpath:
1. Select the toolpaths you want to edit.
2. From the Toolpath menu, select Edit Entry/Exit.
3. Click on the entry/edit point you want to edit.
4. Right-click and select Edit Entry/Exit from the shortcut menu.

5. In the Edit Entry/Exit dialog that displays, edit the entry/exit parameters for the strategy.
6. Check Apply to all Entry/Exit points in selection to apply the changes to all the entry/exit points in the selected toolpaths.
7. Click OK.

Editing Bridges

The Edit Bridges tool allows you to edit individual bridges, move them and change their parameters. It is also possible to insert and delete bridges, and globally change the parameters of all the bridges in the selection.
Bridges are small tabs of material that are left connecting parts which would otherwise be completely severed from the material being cut. After the job has finished cutting, the operator can then
manually cut the bridges to remove the part from the rest of the material.

Working with Toolpaths Page 197

Bridges are displayed as square brackets that ride the line of the toolpath. The area in between the brackets will form the bridge.

Moving Bridges

To move the endpoints of a bridge:
1. Select the toolpath you want to edit.
2. From the Toolpath menu, select Edit Bridges.
3. Click and drag the endpoints of the bridges to the desired locations.

 Bridges cannot be moved on top of the entry/exit points or other bridges.

4. Right-click and select Exit this tool to release the tool.

Editing Bridge Parameters

To edit the parameters of a bridge:
1. Select the toolpaths you want to edit.
2. From the Toolpath menu, select Edit Bridges.
3. Right-click and select Edit Bridge from the shortcut menu.

4. Set the Length and Height of the bridges to the desired values.
5. Check Apply to all bridges in selection to apply the changes to all the bridges in the selected toolpaths.
6. Click OK.
7. Right-click and select Exit this tool to release the tool.

Inserting Bridges

To insert a bridge:
1. Select the toolpaths you want to edit.
2. From the Toolpath menu, select Edit Bridges.
3. Right-click and select Insert Bridges from the shortcut menu.
4. Click on the toolpaths to insert bridges using the current bridge parameters.
5. Right-click and select Exit this tool to exit the Insert Bridges tool.
6. Right-click and select Exit this tool to exit the Edit Bridges tool.

Page 198 Working with Toolpaths

 It is now possible to insert and edit bridges for Open Contour Offset toolpaths.

Deleting Bridges

To delete a bridge:
1. Select the toolpaths you want to edit.
2. From the Toolpath menu, select Edit Bridges.
3. Right-click on a bridge and select Delete Bridge from the shortcut menu.
4. Right-click and select Exit this tool to exit the tool.

Distorting Toolpaths

Menu: Toolpath / Distort Toolpaths

Distorting toolpaths, similar to distorting contours, is a way to introduce an interesting variation into surfaces. When creating 3D surfaces for creative applications, there can be a tendency to obsess about creating ultra-smooth surfaces, and to worry about every visible tooling mark. One solution to this dilemma is to carefully sand away every tool mark in order to create a very smooth surface. An alternative, as argued by our friend in Yarrow, B.C., is to create surfaces that are intentionally textured. There are many ways in EnRoute to achieve textured surfaces, but one relatively new way is to add some distortion directly to the toolpaths. Toolpath distortion can be applied to both Hatch and Island fills. Typically, the distortion should be relatively subtle, but it is a way for surfaces to be created that may require little or no finish sanding, and ultimately create a more interesting design.

Example:
1. Apply an Island Fill toolpath.

Working with Toolpaths Page 199


2. Select the toolpaths and click on the Distort Toolpaths Icon. This will open the Distort
Toolpaths Dialog.

Wavelength – This defines the repetition length of the noise pattern for the toolpaths.

Jitter – This defines the level of smoothness of the noise pattern. Horizontal Amplitude - The size of the distortion in the x-y plane. Vertical Amplitude – The size of the vertical distortion of the toolpaths.

3. Enter the parameters and click Preview to see the toolpaths that will be distorted, make any adjustments to the parameters and then click on Apply.
4. The toolpaths will be distorted. This is a close-up view of the toolpaths.

Creating a straight edge with distorted toolpaths

You may notice that the edges are also distorted. The solution is to add a clean pass to the toolpath.
1. Go into edit the toolpaths and add a clean tool.

2. Edit the width of cut to .20

Page 200 Working with Toolpaths


3. The Clean pass is shown in green. This will allow you to have a straight outside edge.

Another use for this tool is to use the distort tool on the toolpaths that have been applied to a relief to
create a “hand carved” look to the finish.
1. In this example, a rounded relief was created. Island Fill toolpaths were applied. In the parameters, the Vertical Amplitude was adjusted.

2. Click Apply. The toolpaths will be distorted vertically in the Z plane also.


This is a rendering of the toolpaths that were distorted on a relief.
You can come up with many different textures simply by changing the parameters of the distortion.

Working with Toolpaths Page 201

Delete Toolpaths

Menu: Toolpath / Delete Toolpaths

Toolbar: Toolpath / Delete Toolpath

The Delete Toolpaths tool allows you to delete all the toolpaths in a toolpath group. The original contours in the toolpath group will remain.
To delete a toolpath:
1. Select the toolpaths you want to delete.
2. Click Delete toolpaths

Project Toolpaths

Menu: Toolpath / Projecting Toolpaths to a plane

Toolbar: Output / Project Toolpath

This tool provides a method for tipping toolpaths vertically. It is useful for cutting non-horizontal surfaces, and is likely most useful for routing offset and fills. Use this tool to change the height or angle of existing toolpaths.

Project Toolpaths Dialog

Vertical Rotation – The toolpaths can be tipped vertically.

Angle – Check this to set the angle. Height – Check this to set the height.

Apply across selection – Use the entire selection to define the rotation plane.

Rotation Edge – Select the starting side to tip the toolpaths. Vertical Angle – The degree of the angle to assign to the toolpath. Vertical Height – The height of the toolpath angle.

Page 202 Working with Toolpaths

The following image shows a simulation of hatch fill toolpaths that have been rotated down by a few degrees. You can see that one application of this method could be for creating a way to drain an area.

Working with Toolpaths Page 203

Page 204 Working with Toolpaths

9. Previewing Output

Simulating Output in 2D

Menu: Machining / Simulate 2D

Toolbar: Output / Simulate 2D

The Simulate 2D tool allows you to preview the output of your toolpaths in the order they will be sent to the machine. This allows you to review the output before cutting it to make sure that the toolpaths and their order are correct.

To simulate output of your design in 2D:
1. Click Simulate 2D. 

Previewing Output Page 205


2. In the Simulate 2D dialog, use the controls provided to play the simulation. The controls are similar to those on a CD player or tape recorder:

 Hit the up and down arrow keys to speed up and slow down the simulation.







 After any ordering changes are made, be sure to click on the ‘Update Order’ button so that

the changes are reflected in the output and simulation.
3. Click Done to end the simulation.

Page 206 Previewing Output

Simulating Output Using an Orthographic View

Menu: Machining / Simulate Ortho

Toolbar: Machining / Simulate Ortho


The Simulate Ortho tool displays an animated orthographic view of the path each tool will take and the order in which it will cut. If you see that you have made an error in the toolpath or the order of the cut, you have the opportunity to make corrections.
To simulate output of your design using an orthographic view:
1. Click Simulate Ortho

2. In the Simulate Ortho dialog, use the controls provided to play the simulation. The controls are similar to those on a CD player or tape recorder (if you don’t know what a tape recorder is, ask someone old):

 Hit the up and down arrow keys to speed up and slow down the simulation.



Previewing Output Page 207

Changes in Priority Ordering, Tool, Strategy and Sort Method may all be accomplished directly in the 2D Simulation tool so that the effect of any change may be viewed.

 After any ordering changes are made, be sure to click on the ‘Update Order’ button so that the

changes are reflected in the output and simulation.
3. Click Done to end the simulation.

Create Rendered View of Toolpaths

Menu: Machining / Simulate 3D

Toolbar: Machining / Simulate 3D


This tool displays a rendered solid model view of the results of the toolpaths cutting the material. It accurately renders all of the different tool shapes, so you can see the results of both
2D and 3D toolpaths.
To simulate output of your design using a rendered view:
1. Click Create Rendered Simulation of Toolpaths.  This will open the Simulate Options
Dialog.
2. Enter the desire parameters below and then click OK.

Page 208 Previewing Output

 Resolution – Image resolution refers to the spacing of pixels in the image and is measured in pixels per inch. The higher the resolution, the more pixels in the image. Higher resolutions allow for more detail but will take longer to display.

 Material Color – The material color is the color of the relief. You can change this color by clicking on the material color icon and choosing the color from the color chart.

 Cut Color – The cut color has three choices:

 Use tool color – The simulation will show using the colors assigned to each tool type in the preferences section.

 Use Selected color – The selected color is shown to the right. This color can be changed by clicking on the icon and selecting a new color from the chart.

 Use Material color – Select this parameter if you

would like the simulation to be shown using the material color.

 Material Texture – It is now possible to select a bitmap texture to apply to the simulation. If no texture is selected, then the ‘Use material color’ option will use the defined material color for simulation. However, choose from one of the many available wood, metal, and solid surface textures and you can get a new level of realism from the toolpath simulation.

 Use selected contours as mask – Check this to use the selected contours as a mask for the area that you want to simulate.

 Save simulation as relief – The simulation will be saved as a relief. The relief will be placed in the plate.

 Simulation tolerance – The tolerance controls how closely the simulation will display to the relief toolpaths.


3. In the Create Rendered Simulation dialog, use the controls provided to play the simulation.

 Hit the up and down arrow keys to speed up and slow down the simulation.



Previewing Output Page 209

 After any ordering changes are made, be sure to click on the ‘Update Order’ button so that the

changes are reflected in the output and simulation.
4. Click Done to end the simulation.

 Be sure to activate the Rendered View icon. 


Image with rendered view activated. Image without rendered view activated.

Page 210 Previewing Output

10.Configuring the Software

Configuring Machine Drivers

Menu: Setup / Machine Setup

Toolbar: Libraries / Driver Setup

The Machine Drivers dialog is used to select the appropriate driver for your machine, and to configure it, if necessary, to adjust specific parameters. The drivers will typically be located in a folder called NDrivers, located in your program folder. The driver configuration files have a CNF extension, along with a driver file with the same name, with either a PST or DLL extension. Any changes you make to the driver configuration parameters are saved in the CNF file.

 After a driver for your machine is configured, it is not typically necessary to make changes to the driver configuration unless something changes. The exception to this may be changes to the tools loaded in your machine’s tool changer if it is configured with one.

 Another name for a Machine Driver is Post Processor. The concept of a post processor is that it processes output from the design software so that the output is tailored specifically for the machine it is going to drive. This is true for EnRoute too. EnRoute generates toolpath output that is virtually identical, regardless of the machine it will be sent to. The driver, or post processor, then takes that output and reformats it so that it is compatible and tailored for your machine. Even we tend to call them drivers, you can call them post processors and mean exactly the same thing.
To set up a machine:
1. Click Driver Setup

Configuring the Software Page 211

2. Select the driver for the machine from the Current Driver list.
 The Current Driver list displays the drivers which have been selected as active. If the driver for your machine is not in the list, see “Selecting Active Drivers” for instructions on adding the driver to the list.
3. Edit the driver parameters.

Driver Description

Name

The name of the driver file being edited.

Model

The model name of the driver being edited.

Description

The description provides a brief description of the driver, such as what type of driver it is, or specifically what model of machine it has been created for.

Driver Parameters

Width

This provides the width dimension for the machine (typically the X-axis of the machine.

Height

This provides the height dimension for the machine (typically the Y-axis of the machine).

Z Lift

This gives the maximum Z-axis dimension, or thickness, of the machine.

Home

Position

This section defines what type of home definition is being provided, including User DefinedPlateDesign, and Selection. It is most

typically defined as User Defined, which provides a specific location that

is not dependent on elements of the design. The coordinates of the Home Position can also be defined, along with where that corresponds to a location on the machine. After being originally specified in the driver, these values are not typically changed.

Tool Changer

The Tool Changer section specifies whether your machine has a tool changer available, how many tools are present, and which specific tools are available in the turret.

See “Configuring a Tool Changer” for details on setting up a tool

changer.

Drill Bank

The Drill Bank section specifies whether your machine includes a Drill Bank. A drill bank is a separate head that provides an array of drill tools to drill a set of holes using a pre-configured spacing. A typical

application for a drill bank is to bore holes for shelf mounts as part of the

manufacture of cabinet parts.

See “Configuring a Drill Bank” for details on setting up a drill bank.

Page 212 Configuring the Software

Driver Speeds

This category contains a definition of the maximum and minimum speeds that are possible with the current machine. They are based on the physical capabilities of the machine, as well as practical values. This will help ensure that you don’t attempt to define speed values that are not possible, or might damage the machine.

The units used in this category are based on the units that are specified for the machine. Units are specified by machine manufacturers based on the values that are used by their controllers, so it is not recommended to change the speeds unless you know for sure that the change is appropriate.

Spindle

Speed

This provides a default spindle speed that is used if no spindle speed is provided in the output file.

Feed

These are the default feed rates that the machine moves in the X and Y- axes – again, if they aren’t specified in the toolpath output. There are values specified for both ‘Within the material’ and ‘Above the material’. The first refers to cut speeds while the tool is actually cutting material, and the second refers to feed rates as the tool is moving between toolpaths after it has lifted out of the material.

Plunge

These are the speeds that the machine moves in the Z-axis, either as it is moving down into the cut, or moving up out of the cut.

Dwell

It is sometimes desirable for the tool to remain in one position for a short period of time after it has plunged to a depth. This allows the tool to remove chips properly before it begins its cut.

Driver Units

These are the units that are expected by the machine controller for any values it receives. As described above, these values are most often defined by the machine manufacturer and should not be changed by users unless you know for sure that the change is appropriate.

The values are specified for Length, Speed and Time. If you make changes to these values and then decide that the changes are not correct, you can click on the ‘Use defaults’ check box to return the values to their original values.

Communication

Parameters

The communication parameters are used when the software is used to send output directly to a machine. These values are configured to match the parameters specified for communicating with the machine.

These parameters specify how information regarding distance and angles is converted into machine movements.

 Please note that many machine controllers are not designed to receive files directly from the software. If you are not sure how to communicate directly with your machine, check with the manufacturer to find out what communication parameters are appropriate, and whether it is possible to send files using this method.

 Do Not Change these values unless you know for sure that the changes are correct. If the values are specified incorrectly it will make it so that output will be misinterpreted so that distances and speeds will not be correct.

Configuring the Software Page 213

4. Click OK.

Selecting Active Drivers

The list of active drivers in the Current Driver list should list all of the machines commonly used with the software at your location.

Adding an Active Driver

To add a machine to the list of active drivers:
1. Click on the Active Drivers button at the bottom of the Machine Setup dialog.

2. In the Active Drivers dialog, select the manufacturer of the machine from the Manufacturers
list.
3. Click on the arrow on the right end of the manufacturer listing to open a list of their available machine drivers.
4. Select the machine you want to add to the active drivers list from the list of machines.
5. Click OK.

Removing an Active Driver

To remove a driver from the list of active drivers:
1. Click on the Active Drivers button at the bottom of the Machine Setup dialog.
2. Select the driver in the Active Drivers list.
3. Click the Remove button.
4. Click OK.
Removing a driver from the Active Drivers list does not delete it from the Manufacturers list.

Page 214 Configuring the Software

Configuring a Tool Changer

To set up a tool changer:
1. Click the Auto tool changer check box in the machine parameters list of the Machine Setup dialog.

 The Number of Tools and Edit Tools parameters appear after the Auto Tool changer box is checked.

2. Under Edit Tools, click on the Click to Edit text to open the Tool Changer Definition window:

3. To add a tool to the list of tools in the turret:
4. Select the tool that is in the position you want the new tool to occupy.
5. Click Add Tool. The new tool is added to the list in the selected location, and the existing tools are moved down to make room for it.
6. Using the pull-down list for the new tool, select the type of tool that is loaded in that position in the turret.
7. To edit a tool, select a new type of tool from the pull-down list.
8. To move a tool, click twice on the gray row indicator to the left of the tool listing, and then drag it to the new position in the list. The numbering of the tools will be adjusted to reflect the new position.
9. To remove a tool from the list, select that tool and click Remove Tool.
10. To remove all of the tools from the list, click Empty Turret.
11. When you have completed editing the Tool Changer Definition dialog, click OK to save the changes, or Cancel to discard your changes and go back to the Machine Drivers dialog.

 Any changes you made to the number of tools in the turret will be reflected in the Number of tools

parameter.

Configuring the Software Page 215

Configuring a Drill Bank

The Drill Bank supports a Boring head that may be available on your machine. If it is available, you will need to set it up to match the configuration on your machine, in terms of number of drills, arrangement of the drills, and orientation of the drills. In addition to standard vertical drills, EnRoute supports horizontal drills. There are lots of different drill bank configurations, and so it is important to work with your machine manufacturer to make sure you understand the drill numbering and drill arrangement setup you have.
To configure a drill bank:
1. Check the Has drill bank parameter in the machine parameters list in the Machine Setup dialog.
2. Click on Click to Edit to open the Define Drill Bank dialog.

3. Set Number to the number of drill tools that are present on your machine.
4. For each drill tool in your drill bank:
5. Select the type of Drill Tool that is loaded into that position from the pull-down list provided.

 If a tool that is loaded into your machine is not present in the pull-down list, it will need to be created in the Tool Library before you can set up the machine properly. See “Editing the Tool Library” for details.

6. Define the X, Y, and Z location of the tool.
7. Direction - Drill tools are commonly oriented to point down in the z direction (-Z). This is the default orientation in the drill bank. They can be configured to point in the other cardinal directions if that matches the machine configuration. In those cases, EnRoute will determine if any match these orientations and tool selections. If they do, boring commands will be generated for the machine to handle the appropriate horizontal boring tools.

 If horizontal bores are going to be used, it is very important that the machine driver is properly configured for this. Please contact EnRoute Technical Support before attempting to implement a horizontal boring configuration.

Page 216 Configuring the Software

 This location is based on the configuration of the machine you are using. It may be necessary to obtain this information from the manufacturer of your machine. This configuration is used to create the final output, so it is very important that the orientation and position of the tools is defined correctly.

8. After completing the configuration of the drill bank, click on OK to close this dialog. When you click on OK to exit the Machine Drivers dialog, the drill bank configuration you defined will be saved in the driver configuration file.
After you define the layout of your drill bank, you can disable the drill bank in the driver without deleting the layout. Then when you enable the drill bank again, the parameters you defined before will still be present.

 It is important to verify that the driver you are using is capable of using a drill bank. Not all the drivers have been modified to enable them to issue the correct output commands. If you are unsure, please check first with the manufacturer of your machine and then with EnRoute technical support if necessary to find out whether your driver is capable of using drill banks.

Editing the Material Library

Menu: Setup / Material Library

Toolbar: Libraries / Material Library

The Material Library command is used to define the cut speeds for the different types of materials (wood, metal, etc.) that you are routing or engraving. When you use the Define Plate command you can select a Material Type to be associated with the plate. The software will then update the plate information to include the cutting speeds associated with the material you select. Material definitions are written to the MaterialLibrary.ini file located in the folder where the software was installed.

 Some machines and/or drivers may not support the speeds defined in the Material Library. The driver for the machine will override speeds that are defined to be too fast for the machine.

Adding a Material to the Library

Menu: Setup / Material Library

Toolbar: Libraries / Material Library


1. Click Material Library
2. Click New.
3. Enter the parameters for the new material.

Configuring the Software Page 217

Name

The name of the material.

Direction

Select the direction in which the tool will cut across the plate.

Conventional

Left to right milling.

Climb

Right to left milling.

Feed

The speed at which the cutting tool moves through the material

(machining or cutting speed).

Plunge

The speed at which the tool moves down into the material.

Dwell

The amount of time to wait once the cutting tool has moved down into the material. This is used to make sure the tool is all the way into the material before it starts routing or engraving. It is also useful if there is a concern about chip removal.

Spindle

The speed at which the tool will spin.

4. Click Save.

Deleting a Material from the Library

Menu: Setup / Material Library

Toolbar: Libraries / Material Library

1. Click Material Library
2. Select the material from the Name list.
3. Click Delete.
 If you change your mind after deleting a material, click on the Reload button to reload the Material Library from the file. The material is not permanently deleted until the Material Library has been saved.
4. Click Save.

Editing the Tool Library

Menu: Setup / Tool Library

Toolbar: Libraries / Tool Library

The Tool Library stores the list of all cutting tools which have been defined for the software. New tools can easily be added to the tool library as needed.

Page 218 Configuring the Software

Adding a New Tool to the Tool Library

1. Click Tool library

2. Click on the New button.
3. Enter a Tool Name for the new tool.
4. Select the Tool Type that best fits the tool being added.
5. Click OK.
6. Select the newly created tool from the list in the tool library dialog.
7. Edit the parameters of the new tool in the fields at the bottom of the tool library dialog.
8. Save the changes in the tool library (see “Saving the Tool Library” below).

 If you are creating tool definitions for tongue and groove joining tools, create them as end mill tools. Give the tongue bit a diameter equal to the outer diameter of the bit, and the groove bit a diameter equal to its inner diameter.

Deleting a Tool from the Tool Library

Menu: Setup / Tool Library

Toolbar: Libraries / Tool Library

1. Click Tool library
2. Select the tool you want to delete.

Configuring the Software Page 219

3. Click Delete.
4. Click OK.

Saving the Tool Library

Saving the Default Tool Library

To save the default tool library including any changes:
1. Click Save.

2. Check the Save as default tool library box.
3. Click Save.

Saving a Custom Tool Library

A custom tool library may be designed to fit an individual user or a specific job.
1. Open the Tool library.
2. Edit the library so that it contains the tools to be included in this library.
3. Click Save.
4. Enter the name of the new library to be created.
5. Make sure the Save as default tool library box is cleared.
6. Click Save.

Opening a Tool Library

Tool libraries are stored by name in the folder the software was installed into. They may be loaded at any time.
1. Click Tool library
2. Click Open.

Page 220 Configuring the Software


3. Place a check mark in the box of the tool library you wish to open.
4. Select one of the following options:
 Select Open as a New Library box is selected; the tools in the selected library will replace the current entries in the tool library.
 If the Add to current Library box is selected, the tools in the selected library will be added to the current entries in the tool library.
5. Click Open.

 The default tool library is saved in a file called ‘ToolLibrary.ini’. This library is automatically opened when EnRoute loads. If you want specific tools to load every time, then save these tools as entries in the default tool library.

Configuring the Software Page 221

Page 222 Configuring the Software

11.Output to Machine

Setting the Toolpath Order

Menu: Machining / Order

Toolbar: Machining / Order

The Toolpath Ordering dialog allows you to review and edit the order assigned to the toolpath groups in your project. The toolpath order influences the order in which cuts will be made when the project is output.

Ordering Toolpath Groups Manually

To manually adjust the order of the toolpath groups:
1. Click Order
2. Use the horizontal blue arrow buttons to select the toolpaths.

 The selected toolpath is indicated with a bold red number.

3. Use the vertical green arrow buttons to change the cut number of the selected toolpath.
4. When finished, click OK.

 Clicking the horizontal and vertical arrow keys on your keyboard produces the same results as clicking on the blue & green arrow buttons.

Ordering Toolpaths Using the Mouse

To order the toolpath groups manually using the mouse:

Output to Machine Page 223


1. Click Order.
2. Click Manual.
3. Click on each toolpath in the desired order.

Ordering Toolpath Groups Using Sorting Methods

To determine the toolpath order using an automatic sorting method:
4. Click Order
5. Select the sorting method from the Current Sort Method list. The available methods are:

Shortest

The toolpath will be sorted to produce the shortest overall set of toolpaths and movements.

Rows

The toolpaths will be sorted by ordering them into rows starting from the bottom of the plate. Numbering within rows runs from left to right.

Columns

The toolpaths will be sorted by ordering them into columns running from left to right. Numbering within columns runs from bottom to top.

Inside Out

The toolpaths will be sorted by position from the center of the plate to the edges.

Outside In

The toolpaths will be sorted by position from the edges of the plate to the center.

6. Click OK.

Generating Output Menu: Machining / Output Toolbar: Output / Output Options

The goal of virtually all the work you do in the software is creating toolpaths that will then be used to
create an output file, or be sent directly to your router, engraver, or milling machine. After toolpaths have been created, the Output dialog determines which toolpaths will be sent, their order, and a
number of other aspects of the output process.
Click Output

Page 224 Output to Machine


Generating output consists of the following steps:
1. Selecting the machine driver to use when outputting the design.
2. Determining the cutting order of the cuts that make up the design.
3. Selecting output parameters.
4. Outputting the design either to the Output Control Center or a file.
 Sending output can be as simple as opening the Output dialog and then clicking either To File or To Machine. The machine driver, cutting order options and output parameters are there to provide flexibility, not to make the process more complicated.

Selecting the Machine Driver

Click Driver to select the desired machine driver from the Driver Configuration dialog. For details on
the Driver Configuration dialog, see “Configuring Machine Drivers”.

Determining the Cutting Order

The order in which the cuts are made determines the amount of time that it will take to output a finished piece. The software determines the cutting order based on a number of different parameters.

Output to Machine Page 225

 It is not necessary to make any changes to the Ordering Options in order to successfully generate output. The default ordering options are sufficient to generate a high-quality finished piece. They only need to be changed if you want to fine-tune the process.


The ordering options can be set using the Ordering Options list and its related buttons. The buttons cause the list to display ordering options at four different levels:

 Priority is the highest level, and allows you to set the priority levels of the major parameters relative to each other.

 Tool Order sets the relative priority of the various types of tools used in the cutting passes.

 Strategy Order sets the relative priority of the various strategies present in the design.

 Sort Method sets which of the different automatic toolpath sorting methods is in use.

 Small Part First – Check this box if you would like the small parts to cut out first.

 Maintain Grouping – Check this box to treat group objects as one in reference to the cut order.

 Reset Parameters using Preferences  Click here to reset the Parameters using the

Preferences.

 Save Current Parameters to Preferences  – Click here to save the current parameters to the Preferences.

 You can also access the Ordering Options table from the 2D Simulation and Ortho Simulation tools. This allows you to make changes to the ordering options, and then immediately see how they will affect that final output. Changes you make to the ordering options in 2D Simulation and Ortho Simulation will be carried over to the Output dialog.

Setting the Priority

Clicking on the Priority button displays the Priority Order list, which lists the following parameters that can be used to sort the cuts in the design:

Tool The type of cutting too used to make the cut.

Page 226 Output to Machine

Object

The object that the cut forms a part of. An object in this context means a separate piece that will be cut from the plate.

Strategy

The strategy to which the cut belongs.

Bundle

The bundle to which the cut belongs. Bundles are groups of toolpaths that make up a cutting pass.

Pass

The cutting pass to which the cut belongs.

For example, if the priorities are in the order listed above, the cuts will be sorted first by the type of tool they use, then by the individual contours to which the cuts of each tool type belong.

Reordering the Priority List Entries

Entries in the list can be reordered by dragging them up or down in the list. Click on the row header on the left edge of the entry to select it, then drag the entry up or down by the header.

Setting the Priority to Minimize Tool Changes

The default Priority is designed to minimize tool changes in the output:

1.

Tool

2.

Object

3.

Strategy

4.

Bundle

5.

Pass

If your output uses two tools, say a ¼” end mill and a 90-degree conic, all of the toolpaths associated with the first tool would come first, followed by all of the toolpaths associated with the second tool.

Setting the Priority to Cut Each Object Completely Before Continuing

There may be times when minimizing tool changes is not the most important thing to you. For example, the output may contain a number of toolpath groups and it is more important that you cut out each piece one at a time in order to allow you to progress with other work in the shop. In that case, you may want to move ‘Object’ to the top of the priority list. If each object (toolpath group) uses both the ¼” end mill and the 90-degree conic from the example above, there would be a tool change required as each object cuts out. This might increase the number of tool changes significantly, but it would allow you to get finished pieces off the table before the entire job is complete.

Returning to the Default Priority Settings

Click Default Order to return the Priority settings to their default order.

Output to Machine Page 227

Setting the Tool Order

Clicking the Tool Order button displays the Tools list, which lists the priorities assigned to the different tool types used in the design. These settings are used to sort the cuts by tool type in the Tool stage of the sorting process.
For example, if a ¼” end mill tool will be used to cut separate pieces out of the plate, you should make that tool the lowest priority so that any other cuts that need to be made to the piece will be made before it is separated from the plate.

Reordering Tools

Drag the tool entries up and down in the list to assign their priorities. Click on the row header on the left edge of the entry to select it, then drag the entry up or down by the header.

Defining Tools as Unused

Clearing the check box in the Use column to the right of a tool will prevent any cuts that use that tool from being output.

Setting the Strategy Order

Clicking the Strategy Order button displays the Strategies list, which lists the priorities assigned to the different toolpath strategies that appear in the design. These settings are used to sort the cuts by strategy in the Strategy stage of the sorting process.
For example, if you used the same contours to create both male and female Routing Offset toolpaths for an inlay job, you would not want to send both strategies to the machine at the same time, because you would use different material to cut out the male offset than you would for the female offset. So, you would move one of the strategies lower on the list, or even mark it unused.
Drag the strategy entries up and down in the list to assign their priorities. Click on the row header on the left edge of the entry to select it, then drag the entry up or down by the header.

Defining Strategies as Unused

Clearing the check box in the Use column to the right of a strategy will prevent any cuts from that strategy from being output.

Setting the Toolpath Sort Method

Clicking the Sort Method button displays the Sort Methods list, which allows you to select a sorting method that will be used to automatically order the toolpath groups in the design. This is exactly the same as the ordering that can be done using the Order Toolpaths dialog.
If you have already ordered the toolpath groups manually, none of the methods will be checked. If you check a method, it will automatically be applied to the toolpath groups in your design.
For details on the various sorting methods, see “Setting the Toolpath Order”.

Selecting Output Parameters

The following output parameters are available:

Which toolpaths Select one of the following options:

Page 228 Output to Machine

All toolpaths

All toolpaths will be output.

Selected only

Only the currently selected toolpaths will be output.

Depth

Select one of the following options:

All

Toolpaths at all depths will be output.

[Specific Depth]

Only the cut passes at the specified depth will be output. This might be done to finish a job that had been interrupted near its end, for instance.

Orientation

Allows you to output the toolpaths rotated by some increment of 90 degrees. Select 090180, or 270 degrees.

Copies

This option is not implemented at this time. Leave it at 1.

Hold Output

If you are sending the output to a machine through the Output Control Center, this option tells the OCC to hold the output in a queue so that you can send the queue of jobs to the machine when you are ready.

Outputting the Design

Outputting the Design to a File

To output the design to a file:
1. Click To File.
2. In the standard Windows Save As dialog that opens, specify the file name for the output file and click OK.

Output to Machine Page 229

Page 230 Output to Machine

12. 3D Surfaces and 3D Toolpaths

Menu: Surface

Toolbar: 3D Surfaces

Introduction


EnRoute Pro introduces a number of concepts for creating designs and the toolpaths to cut out these designs. All of the previous functions have been oriented around working with two- dimensional (2D) geometry, and then creating either 2D or engraving toolpaths based on the
2D geometry. The Pro functions provide the ability to create three-
dimensional (3D) surfaces and
then create 3D toolpaths associated with these surfaces.
The surfaces you create are compatible with all of the other design elements, and the working
environment is no different than
the environment for the 2D
design. This allows you to easily utilize whatever type of design and toolpath strategy is most appropriate for your application.
This chapter provides a brief introduction to the concept of 3D surfaces, and then subsequent chapters provide detailed information on creating surfaces, manipulating and combining surfaces, and then creating toolpaths to machine these surfaces.

3D Surface Applications

There are certainly countless ways in which 3D surfaces can be utilized in commercial applications. The EnRoute Pro tools are designed primarily as creative tools, making them most useful for applications that require creative designs. This includes woodworking and woodcarving, signs, jewelry, mold-making, and any other application that requires creative design tools.
While EnRoute’s 3D tools can be used to create precise surfaces, their primary application is not considered to be in creating 3D engineered parts for mechanical applications.

3D Surfaces and 3D Toolpaths Page 231

Creating 3D Surfaces

EnRoute provides an array of tools that are used to create 3D surfaces, which are referred to as Reliefs. Reliefs are created and modified using both 2D contours and 3D mesh objects. 2D Contours are used to sweep and spin profiles and cross sections and to extrude shapes to create surfaces. 3D mesh objects can be created in EnRoute, and then applied to reliefs to create a finished surface. EnRoute also allows you to import a number of different file formats, so mesh objects that are created in other applications can be used too.

Creating Output for 3D Surfaces

3D toolpaths are created in much the same way as 2D toolpaths in EnRoute. Hatch Fills and Island Fills are the most common strategy types that are used with reliefs, but other strategies like routing offsets and engraving can also be effectively used to machine a surface. W hen these strategies are used with a relief, some additional parameters become necessary to define how the toolpaths should be created. Otherwise, the process is the same as the processes defined in Chapter 6. Creating 3D toolpaths is discussed in detail in Chapter 19.

Page 232 3D Surfaces and 3D Toolpaths

13.Creating Reliefs

Creating a Relief Menu: Surface / Create Relief Toolbar: 3D Surfaces / Create Relief

The first step in working with surfaces is to create a relief, which can then be modified, and used to
create 3D toolpaths. Click Create Relief. 

This will activate the Precision Toolbar for creating a relief. This dialog provides several parameters that allow you to create and modify reliefs in many different ways. The following sections provide a description of the parameters and how they affect the resulting relief.

Relief Shape

Application Method Relief Options

Relief parameters

Preview Relief angle

Relief Shape

There are three basic shapes available to use for creating a relief. They provide the starting point for creating all of the different surfaces available in EnRoute.

Round 


The round relief uses the relief angle to create a surface that is similar to a flexible surface that has been inflated. It can be used by itself to create rounded organic shapes, and it can also be effectively used to modify other surfaces.

Creating Reliefs Page 233

Beveled 

Flat 

The beveled option creates a surface that is similar to the shape of a surface that is created by using Pyramid toolpaths. EnRoute creates this type of surface by extending a flat surface up from the perimeter of the selected contour to the
‘center’ of the shape where it meets a surface extended up from the other side of the shape. This is a complex operation, but EnRoute handles all of the computations, and all that is required is to provide the angle of the surface.

The flat option is used to create a simple flat surface. This option is used primarily as a means of creating a surface that can then be modified using other relief tools such as the sweeping and extrusion tools. By specifying a Height of 0.00, the flat surface is created at the height of the contours. If a height is specified, then the flat surface is created above that contours by that amount, as shown in the adjacent image.

Relief Options

The relief options allow you to modify the basic relief shapes to create different surface shapes. So, for a given relief shape, such as Round, you have the following four different options that allow you to modify how that shape is created.

Normal

This is the default option that is described in the previous Relief Shape section. The key distinguishing characteristic of this option is that the relief shape, either round or beveled, is created based on the specified angle. The height of the relief is defined based on the width of the surface at each location. As the surface becomes wider or narrower, its height is greater or smaller accordingly. The following images illustrate this option for both round and beveled relief shapes.


Page 234 Creating Reliefs

Constant Height


The Constant Height option changes the way that round and beveled shapes are created. Instead of using a relief angle to define the relative steepness of the surface, you define a height for the relief, and the surface is created to match that height. This option creates a surface that can be described as more mechanical looking. The way that it varies from the Normal option is most apparent in areas where different parts of a relief merge together. The following two graphics illustrate this option.

Scale to Height

This option is a variation of the Normal option. Using this option first creates the surface using the Normal option, and then the relief is scaled vertically so that its height matches the specified height. It comes in handy when you want to create normal relief, but you also want it to be a specific height. It is also a way to create surfaces that are subtly different by specifying different angles and the same height.
The following images show a relief that was created using the Scale to Height option. The relief on the left used a relief angle of 85 degrees and the relief on the left used an angle of 15 degrees. The height of each relief is the same, but the shape of each relief is different because of the different angle.

Creating Reliefs Page 235

Limit to Height

This option is also a variation of the Normal option. The relief is first created using the normal option, and then it is cut off at the specified height. It is useful is cases where you want to create a relief that has rounded or beveled profile up to a certain height, and then a flat top surface.
The following graphic shows a relief that uses a rounded shape that is limited to a height that is about half the height that it would have been if it wasn’t limited. This is an option that will not likely be used very often, but it can be useful for specific applications.

Application Method

The application method defines how the application of a relief modifies the surface. The terms for each option are descriptive of how the relief will be modified.

 The Application Method is a concept that is common throughout all of the relief creation tools. The way that the concept is used is consistent for each of these tools.

Add 

This is the option that will likely be used most often. It is used to create a raised relief. If you are modifying an existing relief, the surface will be raised using the selected contours and parameters specified for the relief.
The following image shows an example of a relief created using the Add option.
In this image, the top surface was created using the Add option on an elliptical contour.
The bottom surface was created by adding the letters to an existing relief surface. This was accomplished by selecting the relief and the contours for the letters and then applying the relief function.

Page 236 Creating Reliefs

Subtract 


This option is used to create a recessed relief. It can either be applied to contours to create new recessed reliefs, or using contours to modify an existing relief. If an existing relief is to be modified, it should be selected along with whatever contours are to be used to modify it.
The following graphic shows the effect of the subtract option.
The top portion of the image shows individual contours that were used to create individual reliefs. The bottom elliptical relief was modified using the same contours and the subtract option.

Merge Highest 

This option is most effective when it is used to modify an existing relief. It can be used when creating a new relief, but the effect will be the same as the Add option. When it is used to modify a relief, the new portion of the relief only modifies the existing relief where it is higher than the existing relief.

This is best illustrated with a simple example, as shown in the following image. In this example, the top letter was created
using the Merge Highest option. Notice that it
is the same as if it was created using the Add option.
The bottom portion of the image shows an existing elliptical relief that was modified using the same contour. The key thing to notice is that the relief was only modified where the relief created by the new contour was taller than the existing relief.
 Note that if you are creating a new relief, the AddMerge Highest and Replace options will all create the same result.

Creating Reliefs Page 237

Merge Lowest 

The Merge Lowest option is similar to Merge Highest, except that a relief is only modified where the new relief is lower than the existing relief. This option is a little less intuitive than the Merge Highest option. Essentially, wherever a relief would not be modified by a Merge Highest option, it would be modified by a Merge Lowest option.
The following graphic demonstrates how a contour can be used to modify an existing relief using this option.

The top portion of the image shows the result of using this option to create a new relief. Note that the result is a flat relief. This result is caused by the fact that a flat surface is the lowest surface over the entire area of the relief, so that is the result. This indicates that this option should not be used when creating new reliefs.
The bottom image demonstrates the result of modifying an existing relief using the same contour. The relief is modified only in areas where the new profile is lower than the existing relief. In areas where the new profile is higher than the existing relief, the existing relief is not modified. This option will likely be appropriate only in special applications.
 sing the Merge Lowest option to create a new relief will result in a flat surface being created.

Replace 


The Replace option is also used primarily to modify an existing relief. If it is used to create a new relief, the result is the same as the Add option. When it is used to modify a relief, the applied profile takes the place of the existing relief wherever the new profile overlaps the existing profile.
The following image shows the result of the Replace option used to create and modify a relief.
In this image, the top letter was created as a new relief. The bottom relief was modified using the contour of the letter. You can see that the relief created by the letter takes the place, or replaces, the existing relief.

Page 238 Creating Reliefs

Relief Parameters

Height

The Height parameter is used to define the height of the relief that is created when appropriate for the selected relief option. A height is used for the Constant Height, Scale to Height, and Limit to Height options. The entered value uses the active units.
EnRoute enables and disables this parameter based on the Relief Option selected, so when it is not necessary for a value to be entered, this parameter is disabled. When the Normal option is selected, the relief is defined using the angle parameter, so the height is not needed.

Resolution

This parameter is used by EnRoute when a new relief is being created with this command. The Resolution is specified in ‘dots per inch’ (dpi) regardless of the units that are selected. So, even if you are operating EnRoute with active unit of millimeters, this parameter is still specified in dpi.
The resolution of the relief defines the size of the grid units that make up the relief. A relief is a gridded surface and when a relief is created, it is necessary to define how large each grid unit should be. If a resolution of 100 dpi is selected, then each grid unit will be 1/100 inches wide and tall. Therefore, the level of detail for the information on that relief will be limited to 0.01 inch. This resolution is typically adequate for most surfaces in EnRoute, unless you are creating a small object that requires more detail

The thing to remember is that reliefs in your drawing require memory that is directly related to the size of the relief and its resolution. As you increase the size of a relief, it requires more memory. If two reliefs are the same size and one relief is 100 dpi and the other 200 dpi, the second relief will require four times the amount of memory as the first. You can see that this is an important consideration when defining a relief. In general, you should define as low a resolution for a relief as will accommodate the level of detail for that relief.

Creating Reliefs Page 239

Base

The Base parameter allows you to move the relief surface up, creating vertical sides on the portion of the relief that you are modifying. If you are creating a new relief, a base dimension will create vertical sides around the perimeter of the relief.
This parameter will likely be most useful when you are modifying an existing relief and would like to include vertical sides around the portion you are modifying. If you are creating a new relief and want it to have vertical sides, it is possible to move it vertically to position it in the plate so that when it is cut out the parts will have the correct height of vertical edges.
The following image shows two reliefs that include base dimensions. The top relief was created with a rounded profile and a base dimension to create the vertical sides on the letter. The bottom image was a relief that was modified to add the letter with the base dimension.

Page 240 Creating Reliefs

Angle

The Angle parameter is used to define Round and Beveled reliefs when the Normal relief option is selected. Both positive and negative angles may be used between 0 and 90. With beveled reliefs, the angle defines the angle of the bevel. With round reliefs, the angle defines the angle of a line tangent to the circle that defines relief. If an angle of 90 degrees is used with a round relief, a semi -circle is used to create the relief.
The preview drawing in the dialog shows a small preview of the relief shape based on the angle that is defined. The angle can be entered directly into the edit box, or the spinner arrows can be used to define the angle, and there is also a slider bar that can be used to define the angle.
The following graphic show how different effects can easily be achieved just by using different angles. Relatively flat surfaces such as those on the left are created by using small angles, and more dramatic surfaces are created by using larger angles such as those on the right.

 When the Constant Height relief option is selected, the Angle parameter is disabled because it is not used in this option.

Creating Reliefs Page 241

Using the Relief Dialog

Now that the options and parameters have been introduced in the previous sections, the next task is to use the Relief creation tool to create and modify a relief. This section includes a presentation of the steps required to create a relief using just this tool.
The following graphic shows some simple 2D artwork that is used to create the relief example. To repeat this example, you can create an ellipse and some contour artwork similar to the ‘fleur’ shown in this example.


1. Create your 2D artwork.
In this example, create an ellipse and center artwork
like the fleur. The ellipse
is approximately 8 inches tall by 6.5 inches wide (200mm x 116mm).

2. Select the ellipse and offset it with a 0.5 inch inline and a 0.01 inch outline.

Page 242 Creating Reliefs

3. Select the original ellipse.
This will be used to create the base relief.

4. Click on the Create Relief icon, or select the Surface menu and Create Relief.


5. Select the Flat relief option.
6. Select the Add option. 

7. Define the parameters to
Height = 0.00, Base =
0.00 and Resolution = 100 and select the Normal relief type.

8. Click Apply to get the following result. Click the Rendered Icon  to toggle to the rendered view of the relief on and off.
9. Now select the relief and the two offset ellipses that were created in Step 2. (Toggle the rendered view  off in order to select the ellipses).

10. Select the Round relief option.

11. Select the Add Option and leave the relief type on Normal.

Creating Reliefs Page 243


12. Set the Angle to 50 degrees.

13. Click Apply to create the next step in the finished relief.
14. Now select the relief and the smaller ellipse.

15. Select the Round relief option.

16. Select the Subtract
application method.
17. Set the Angle to 30 degrees.

18. Click Apply to create the next portion of the relief.
19. Now select the relief and the center artwork.

Page 244 Creating Reliefs

20. Select the Beveled option. 

21. Select the Add application method.

22. Define the parameters to
Height = 0.30, Base =
0.00 and select the

Constant Height relief

type.

23. Click Apply to create the finished relief.
 As you can see, using just the Create Relief tool provides some very powerful capabilities for creating finished reliefs in EnRoute. The following chapters discuss the many other tools EnRoute provides for creating and modifying surfaces. The concepts presented in this chapter regarding adding and subtracting reliefs are consistent throughout each of the other functions.

Creating Reliefs Page 245

Page 246 Creating Reliefs

14.Revolutions and Extrusions

Introduction

The previous chapter provides the basic tools for creating relief surfaces. This chapter describes additional tools that increase your ability to define intricate surfaces. These tools use revolutions and extrusions to create meshed objects and modify selected relief surfaces.
When modifying reliefs, the concepts presented in the previous chapter regarding application methods work identically with these tools. The primary new concept with these tools is that EnRoute uses wizards to prompt you regarding the selection of appropriate contours to use to define how the function is to be applied. After you understand how they work, they provide a flexible method for completing each function.

Revolve

Menu: Surface / Create Surfaces / Revolve

Toolbar: 3D Surfaces / Revolve


The Revolve tool allows you to use one or more contours to revolve around an axis to either modify a relief or to create a new mesh object, as illustrated in the following image.

Relief Surface
Mesh Object

Revolutions and Extrusions Page 247

Revolve Dialog

Selecting the Revolve icon  , or selecting the Surface menu and then Create Surface and Revolve, will activate the Revolve dialog. This dialog allows you to select the appropriate options and parameters required to create the new surface.
The revolve dialog provides two sets of parameters depending on whether you have selected the option of creating a mesh object, or any other application method for modifying an existing relief. If you select an application method for modifying a relief, the following dialog is presented.

Relief Options

Relief parameters

Application Method to modify the selected relief

Angles for revolution Wizard prompts

Mesh Parameters

Application Method to create a mesh object

Application Method

All of the options for applying the results of the revolve operation are the same as the options described in the previous chapter on relief creation. The options for Add, Subtract, Merge Highest, Merge Lowest, and Replace all apply to the situation where the revolution is to be applied to an existing relief. For this to be possible, it is necessary to select the relief to be modified before starting the Revolve command.
The right-most application method option  allows you to create a mesh object with the Revolve command. As shown in the dialogs above, when this option is selected, the parameters required for the command are different than when a relief is to be modified. When this option is selected, the parameters change, providing space to enter the number of slices and stacks that will make up the new object. These are described below, and the rest of the revolve command is the same whether you are modifying a relief or creating a new mesh object.

Page 248 Revolutions and Extrusions

Relief Options

These options function similar to how they work in the relief creation tool. In this case you have three options, Normal, Scale to Height, and Limit to Height.

 Normal – The revolved surface is created just as the selected profile and axis define it, without any vertical scaling.

 Scale to Height – The revolved surface is scaled to match the height parameter as it is applied to the relief. This allows you to create a revolved surface and scale it in one step.

 Limit to Height – The revolved surface is limited in height by the height parameter. If a portion of the revolved surface extends above this height, it is truncated before it is applied to the selected relief.

Relief Parameters

The relief parameters of Height and Base are available when modifying a relief.

 Height – This value defines the height if either the ‘Scale to Height’ or ‘Limit to Height’ relief option

is selected.

 Base – This value allows you to define a base height that can be added to the revolved surface as it is applied to the selected relief.

Angles for Revolution

The Start Angle and Finish Angle define the portion of a complete 360-degree revolution that will be completed. A complete revolution would have a start angle of 0 degrees and an end angle of 360 degrees. A half revolution would use a start angle of 0 degrees and an end angle of 180 degrees.
The following front view of a revolved mesh object illustrates the start and finish angles. This object used a start angle of 45 degrees and an end angle of 135 degrees.

End Angle

Start Angle

Revolutions and Extrusions Page 249

Wizard Prompts

The Revolve tool requires more than one step in order to complete it. This portion of the dialog contains an area that contains a prompt that tells you the next step required in order to complete the function. It also contains buttons that allow you to move from step to step, back up a step, back up to that start of the function, execute the function, or exit the function.
The first prompt asks you to ‘Select the contours to be revolved.’ After selecting one or more contours, you can select the next step button, which will then prompt you to ‘Select the axis of revolution (Optional)’. At this stage, you can either select a contour that will serve as the axis of revolution, or select the execute button.
Following is a listing of each of the wizard buttons and its function.

Start

Return to the start of the command

Back

Go back one step

Next

Go to the next step

Execute

Execute the function

Cancel

Cancel the function

Mesh Parameters

When the mesh option is selected, it activates parameters that are specific to this option. They include the number of Slices and the number of Stacks that are to be used to create the mesh object.
A mesh object is composed of triangles, or facets, that make up its surface. It is necessary to instruct EnRoute regarding how many of these facets should be used to construct the object. The number of Stacks is the number of sections that are used along the length of the profile that is revolved. The Slices value is the number of sections that are used between the start and end angles.
The following graphic illustrates this concept. This object was created to resemble a pie, with each of the pieces of the pie representing a slice, and the facets that make up each piece of the pie representing the stacks. The profile of a piece of the pie was revolved around the center of the pie.

Page 250 Revolutions and Extrusions

Modify a Relief Surface

The first option is to use the Revolve tool to modify an existing relief surface. The advantage of this option is that it takes care of creating the revolution and applying it to the relief in one step. Also, it automatically takes care of creating a smooth surface without you having to specify any additional parameters. The limitation of this option is that it does not allow you to modify the revolved surface before applying it to the relief.
The following steps lead you through the process of creating a revolution to modify an existing relief.

 

1. Create your 2D artwork. In this example, create an ellipse, a vertical line, and a profile like the one shown. The ellipse is approximately 8.5 inches tall by 7.75 inches wide (215mm x

195mm).

 

2. Select the ellipse and use it to create a round relief using an angle of 25 degrees.

 

3. Select the relief, and then select

Revolve , or select the Surface

menu and then Create Surface/Revolve.

 
 

4. Click on Add to select that option

 

5. Select the Normal application method

 
 

6. Define a Start Angle of 0.0 and an End

Angle of 180.00

 
 

7. Click to select the profile contour you want to revolve, and then click Next Step in the wizard.

Revolutions and Extrusions Page 251

8. Click on the vertical contour to identify the axis of revolution. This step is optional.

9. Click on the Execute button to complete the command.

10. The following shows a rendered perspective view of the resulting relief.

Create a Mesh Surface

Creating a mesh surface using the Revolve tool is almost the same as using this tool to modify a relief. Key differences are that it is not necessary to identify a relief to modify, you need to select the mesh object option, and then you need to define the mesh parameters of slices and stacks. The resulting mesh object can then be used to modify a relief, but first you can scale, rotate and position the object so that when you add it to a relief it has the effect you need. You can also define the number of slices and stacks, using the faceted nature of the object to your advantage.
The following steps illustrate the method of creating a mesh object using the Revolve tool.

1. Create your 2D artwork. In this example, create a vertical line and a profile like the one shown.

2. Select Revolve , or select the Surface menu and then Create Surface/Revolve.

 

Page 252 Revolutions and Extrusions

3. Click on Mesh to select that option.

4. Define Slices = 32 and Stacks = 24

 

5. Define a Start Angle of 0.0 and an

End Angle of 180.00

 

6. Click to select the profile contour you want to revolve, and then click Next Step in the wizard.

7. Click on the vertical contour to identify the axis of revolution. (This step is optional.)

8. Click on Execute to complete the command.

9. The following shows the mesh object like the one that will be created. This object can then be scaled and rotated, and then used to modify a relief.

Spin

Menu: Surface / Create Surfaces / Spin

Toolbar: 3D Surfaces / Revolve / Spin


The Spin Tool is quite similar to the Revolve Tool that was explained in the previous section. The primary difference is that in the Spin tool, the selected contours are spun around the Z-axis, located at a center of rotation by the user. In addition, there are a couple of options that are introduced in the spin tool that give you some additional control over the shape of the resulting surface.
You have the option to apply a spin directly to a relief, or to create a mesh surface. As with this option in other tools, when the spin is applied to a relief it is automatically smoothed and when you create a mesh surface, the result is an object that can be modified further before applying it to a relief.

Revolutions and Extrusions Page 253

With some careful planning, the spin tool can be used to create intricate and interesting surfaces.

Spin Dialog

Selecting the Spin icon , or selecting the Surface menu and then Create Surface and Spin, will activate the Spin dialog. This dialog allows you to select the appropriate options and parameters required to create the new surface.
The Spin dialog provides two sets of parameters depending on whether you have selected the option of creating a mesh object, or any other application method for modifying an existing relief. If you select an application method for modifying a relief, the following dialog is presented.

Relief Options

Relief parameters


Angles for spin

Application Method to modify the selected relief

 Wizard prompts


If you select the Application Method for creating a mesh object, the dialog is changed to allow you to enter the proper parameters for the mesh, and shown below.

Mesh Parameters

Angles for spin

Wizard prompts

Application Method to create a mesh object

Page 254 Revolutions and Extrusions

Application Method

All of the options for applying the results of the spin operation are the same as the options described in the chapter on relief creation. The options for Add, Subtract, Merge Highest, Merge Lowest, and Replace all apply to the situation where the revolution is to be applied to an existing relief. For this to be possible, it is necessary to select the relief to be modified before starting the Spin command.
The right-most application method option  allows you to create a mesh object with the Spin command. As shown in the dialogs above, when this option is selected, the parameters required for the command are different than when a relief is to be modified. When this option is selected, the parameters change, providing space to enter the number of slices and stacks that will make up the new object. These are described below, and the rest of the Spin command is the same whether you are modifying a relief or creating a new mesh object.

Relief Options

These options function similar to how they work in the relief creation tool. In this case you have three options, Normal, Scale to Height, and Limit to Height.

 Normal – The new spin surface is created just as the selected profile and other options define it, without any vertical scaling.

 Scale to Height – The new spin surface is scaled to match the height parameter as it is applied to the relief. This allows you to create a surface and scale it in one step.

 Limit to Height – The new spin surface is limited in height by the height parameter. If a portion of the new surface extends above this height, it is truncated before it is applied to the selected relief.

Relief Parameters

The relief parameters of Height and Base are available when modifying a relief.

 Height – This value defines the height if either the ‘Scale to Height’ or ‘Limit to Height’ relief option

is selected.

 Base – This value allows you to define a base height that can be added to the revolved surface as it is applied to the selected relief.

Spin Angles

The Start Angle and Finish Angle define the portion of a complete 360-degree spin surface that will be completed. A complete revolution would have a start angle of 0 degrees and an end angle of 360 degrees. A half revolution would use a start angle of 0 degrees and an end angle of 180 degrees.
The following top view of a mesh object illustrates the start and finish angles. This object used a start angle of 45 degrees and an end angle of 135 degrees.

Revolutions and Extrusions Page 255

End Angle

Start Angle

In addition to defining the start and end angles using the dialog, the Spin tool also allows you to interactively define this angle by clicking and dragging on the circle that is used to define the center of the spin. This circle is shown in the image below.

Click and drag to change the spin angle

Mesh Parameters

When the mesh option  is selected, it activates parameters that are specific to this option. They include the number of Slices and the number of Stacks that are to be used to create the mesh object.
A mesh object is composed of triangles, or facets, that make up its surface. It is necessary to instruct EnRoute regarding how many of these facets should be used to construct the object. The number of Slices is the number of sections that are used along the length of the profile that is spun. The Stacks value is the number of sections that are used between the start and end angles.
The following graphic illustrates this concept. The same profile was used to create these objects. The object on the left was created using more slices and fewer stacks, and the object on the right was created using fewer slices and more stacks.

Slices = 24

Stacks = 8

Slices = 8

Stacks = 24

Page 256 Revolutions and Extrusions

Wizard Prompts


The Spin tool requires more than one step in order to complete it. This portion of the dialog contains an area that contains a prompt that tells you the next step required in order to complete the function. It also contains buttons that allow you to move from step to step, back up a step, back up to that start of the function, execute the function, or exit the function.

Prompt

Buttons to change steps

The following table lists the prompts in the Spin tool, along with an explanation the appropriate action.

Select the contours to spin

This is the first step, and you are prompted to select the contours you want to use as the profiles for the spin. Note that you can select more than one profile contour to use.

Select the height control curve

(Optional)

This optional step allows you to select another curve to use to modify the height of the spin surface.

Select the width control curve

(Optional)

This optional step allows you to select another curve to use to modify the width of the surface as it is spun around the center axis.

Following is a listing of each of the wizard buttons and its function.

Start

Return to the start of the command

Back

Go back one step

Next

Go to the next step

Execute

Execute the function

Cancel

Cancel the function

Revolutions and Extrusions Page 257

Height Control Curve

The optional second step of the wizard gives you the option to identify a curve that will modify the shape of the spun surface as it is created. This provides a creative tool that allows you to create a surface that can be quite different that the one you would get without this option.
The following graphic shows two surfaces created using this tool. The surface on the left was created using a Height Control Curve. The surface on the right used the same profile without using this step.

The next graphic shows the contours that were used to create the surfaces above. The Height Control

Curve is a contour in EnRoute that is used to define the shape of how the surface is to be modified.

After selecting the Height Control Curve, the Influence Line is automatically drawn along the bottom of the curve. This line determines the amount of influence the Height Control Curve will have on the spun surface. As you interactively drag the Influence Line away from the Height Control Curve, the curve will have less influence on the spun surface as it is created.

Height Control Curve

Influence line. Click and drag it to change the amount of influence of the Height Control Curve

Spin Center/Spin Angle Circle

Profile contour

Page 258 Revolutions and Extrusions

Width Control Curve

The optional third step of the wizard works similarly to the second step, except now you have the option of choosing a curve that will affect the width of the spun surface.
The following graphic shows two spun surfaces. The surface on the left was created using a Width

Control Curve, and the surface on the right did not use this option.


The optional steps to modify the surface can be used separately, or together to create surfaces. The following image shows surfaces that were created using the same method, except for the use of these optional steps.

With both options

With Width

Control Curve

With Height

Control curve

Just the profile

Modify a Relief Surface


This section provides a table with the steps necessary to create a spin surface using the option of modifying an existing relief.
1. Create the 2D artwork. In this example, create a circle and a contour you want to use as the profile for the spin.

Revolutions and Extrusions Page 259

2. Select the circle and use it to create a flat relief.

3. Select the relief, and then select Spin , or select the Surface menu and then Create Surface/Spin.

4. Click on Add to select that option.

5. Select the Normal application method.

 

6. Define a Start Angle of 0.0 and an

End Angle of 360.00.

 

7. Click and drag the blue centering circle to define the center point for the spin.

8. Click to select the profile contour you want to spin, and then click the Next Step icon in the wizard.

9. If you want to include either of the optional steps, you can identify a Height Control Curve and/or a Width Control Curve.

10. Click on the Execute button to complete the command.

Page 260 Revolutions and Extrusions

11. The following shows a rendered top view of the resulting relief.

Create a Mesh Surface

This next set of steps shows how to create a mesh object using the Spin command. It also demonstrates the two optional steps for selecting a Height Control Curve and a Width Control Curve.

1. Create your 2D artwork. In this example, create the contour you want to use as the profile for the spin, and also create two additional curves to use as the Height Control Curve and the Width Control Curve.

2. Select the relief, and then select the Spin icon, or select the Surface menu and then Create Surface/Spin.

3. Click on the Mesh icon to select that option.

4. Define Slices = 24 and

Stacks = 72.

 

5. Define a Start Angle of 0.0 and an End Angle of 360.00.

 

Revolutions and Extrusions Page 261

6. Click and drag the blue centering circle to define the center point for the spin.

7. Click to select the profile contour you want to revolve, and then click the Next Step icon  in the wizard.

8. At this step, you are

prompted to select the Height

Control Curve.

9. Click on the Height Control Curve. A red influence line is drawn; click and drag this line down to reduce the influence of the Height Control Curve.

10. Click on the Next Step icon  to move to the next step in the wizard. You will

be prompted to select a width control curve.

11. Click on the Width Control Curve. A gray influence line is drawn; click and drag this line down to reduce the influence of the Width Control Curve.

12. Click on the Execute button to complete the command.

Page 262 Revolutions and Extrusions

13. An object similar to the one shown to the right will be created.

14. This image shows a rendered view of the object. You can adjust the number of Slices and Stacks to change the

‘smoothness’ of the object.

Extrude

Menu: Surface / Create Surfaces / Extrude

Toolbar: 3D Surfaces / Extrude


The Extrude tool provides a means to extrude a profile, or profiles, along a path to either modify a relief or create a mesh object. While the previous two tools are used to spin and revolve profiles around a central axis, this tool creates its surface along a path. Otherwise, it is very similar to the Spin and Revolve tools.
Two options that provide some additional flexibility include the ability to change the size of the profiles as they are extruded, and the ability to rotate the profiles as they are extruded. These options allow you to create some interesting surfaces, as will be demonstrated in the examples in this section.
The image below shows an extrusion where the profile was rotated as it was extruded.

Revolutions and Extrusions Page 263

Extrude Dialog

Selecting the Extrude icon  , or selecting the Surface menu and then Create Surface and Extrude, will activate the Extrude dialog. This dialog allows you to select the appropriate options and parameters required to create the new surface.
The Extrude dialog provides two sets of parameters depending on whether you have selected the option of creating a mesh object, or any other application method for modifying an existing relief. If you select an application method for modifying a relief, the following dialog is presented.

Relief Options

Relief parameters

Miter Option

Scale and Rotation

Application Method to modify the selected relief

Profile Placement

Wizard prompts

If you select the Application Method for creating a mesh object, the dialog is changed to allow you to enter the proper parameters for the mesh, and shown below.

Mesh Parameters

Miter Option

Scale and Rotation

Profile Placement

Wizard prompts

Application Method to create a mesh object

Page 264 Revolutions and Extrusions

Application Method

All of the options for applying the results of the extrude operation are the same as the options described in the chapter on relief creation. The options for Add, Subtract, Merge Highest, Merge Lowest, and Replace  all apply to the situation where the revolution is to be applied to an existing relief. For this to be possible, it is necessary to select the relief to be modified before starting the Extrude command.
The right-most application method option  allows you to create a mesh object with the Extrude command. As shown in the dialogs above, when this option is selected, the parameters required for the command are different than when a relief is to be modified. When this option is selected, the parameters change, providing space to enter the number of slices and stacks that will make up the new object. These are described below, and the rest of the Extrude command is the same whether you are modifying a relief or creating a new mesh object.

Relief Options

These options function similar to how they work in the relief creation tool. In this case you have three options, Normal, Scale to Height, and Limit to Height.

 Normal – The new extruded surface is created just as the selected profile and other options define it, without any vertical scaling.

 Scale to Height – The new extruded surface is scaled to match the height parameter as it is applied to the relief. This allows you to create a surface and scale it in one step.

 Limit to Height – The new extruded surface is limited in height by the height parameter. If a portion of the new surface extends above this height, it is truncated before it is applied to the selected relief.

Scale and Rotation

These options allow you to modify the extruded surface. The Scale factor identifies the proportion that the profile is to be scaled along the length that it is extruded. If you don’t want to scale the profile, then define a value of 1.0. If you want to reduce the profile size by one half, then define a value of 0.5 for the Scale factor.
The following image shows an object created using a circle extruded along the length of a semi-circle. The scale factor for this extrusion was 0.25.

Revolutions and Extrusions Page 265

The Rotation parameter defines the number of times that the profile will be rotated as it is extruded. A value of 1.0 will cause the profile to be rotated 360 degrees over the length of the extrusion. This is illustrated in the following graphic that was created by extruding a square profile along a semi-circle while rotating it one time.

Profile Placement

The Profile Placement buttons  allow you to position the extruded profile in nine different positions relative to the path. Each button indicates a position on the selection of profiles that will be extruded. This position is the location that the profiles will be places as they are extruded around the path.
If you select the lower left button, then the lower left corner of the selected profile is where it is located as it is extruded around the path. The following graphic shows a top view of set of simple extrusions that were each created using the same profile and the same path, with just the Profile Placement button changing for each object. The top view and right view show how the objects were created both horizontally and vertically.


Page 266 Revolutions and Extrusions

Relief Parameters

The relief parameters of Height and Base are available when modifying a relief.

 Height – This value defines the height if either the ‘Scale to Height’ or ‘Limit to Height’ relief option

is selected.

 Base – This value allows you to define a base height that can be added to the extruded surface as it is applied to the selected relief.

Mesh Parameter

When the mesh option  is selected, it activates parameters that are specific to this option. They include the number of Slices and the number of Stacks that are to be used to create the mesh object.
A mesh object is composed of triangles, or facets, that make up its surface. It is necessary to instruct EnRoute regarding how many of these facets should be used to construct the object. The number of Slices is the number of sections that are used along the length of the profile that is spun. The Stacks value is the number of sections that are used along the extrusion.
The following graphic illustrates this concept. The same profile was used to create these objects. The object on the left was created using more slices and fewer stacks, and the object on the right was created using fewer slices and more stacks.

Revolutions and Extrusions Page 267

Modify a Relief Surface

This section provides a table with the steps necessary to create an extruded surface using the option of modifying an existing relief.

1. Create the 2D artwork. In this example, create an ellipse and then outline it. Then place four overlapping circles and weld then together. After they are welded, if there is a center hole, ungroup the object and delete the center.

2. Select the ellipse and use it to create a flat relief.

3. Select the relief, and then select Extrude  , or select the Surface menu and then Create Surface/Extrude.

4. Click on Add to select that option.

5. Select the Normal application method.

 

6. Define Scale = 1.00 and

Rotations = 0.0.

 

7. Make sure that the Miter option is unchecked, and click on the center Profile Placement button.

Page 268 Revolutions and Extrusions

8. Click to select the profile contour you want to extrude, and then click Next Step in the wizard.

9. Click on the original ellipse to use as the path for the extrusion.

10. Click on the Execute button to complete the command.

11. The following shows a rendered top view of the resulting relief.


Revolutions and Extrusions Page 269

Create a Mesh Surface

The example in this section demonstrates how to create a mesh object by extruding a profile.

1. Create the 2D artwork. Create a small profile as shown in the upper left, and then create a path similar to the one shown. It is not necessary to duplicate this shape precisely. It was created by drawing simple rectangles and then welding them together.

2. Select the Extrude  icon, or select the Surface menu and then Create Surface/Extrude.

3. Click on the Mesh icon to select that option.

4. Define Slices = 24 and Stacks =

150.

 

5. Define Scale = 1.00 and

Rotations = 6.0.

 

6. Make sure that the Miter option is checked, and click on the center Profile Placement button.

7. Click to select the profile contour you want to extrude, and then

click the Next Step icon  in

the wizard.

Page 270 Revolutions and Extrusions

8. Click on the original ellipse to use as the path for the extrusion.

9. Click on the Execute button to complete the command.

10. The following shows a top view of the resulting object.


Revolutions and Extrusions Page 271

Sweep Two Rails

Menu: Surface / Create Surfaces / Sweep Two Rails

Toolbar: 3D Surfaces / Revolve / Sweep Two Rails


The Sweep Two Rails tool provides another method of using profile contours to either modify an existing relief or create a new mesh surface. The rails are open contours that provide a path for the right and left edges of cross section contours to follow as the profiles are used to create an extruded surface.
This tool is very flexible, and can be used to create a wide range of surfaces. It is also very useful when used to modify existing relief surfaces, particularly when the relief surface acts as a stencil to extract the swept surface. This will be illustrated by the examples later in this section.
The following simple mesh surface demonstrates the result of sweeping a semi-circle and an angled contour along two straight rails. This demonstrates how EnRoute transitions between cross sections along the length of the rails.

This next image demonstrates a more complex surface that was created by using curved rails and curved cross sections.

Page 272 Revolutions and Extrusions

Sweep Two Rails Dialog

Selecting the Sweep Two Rails icon  , or selecting the Surface menu and then Create Surface and Sweep Two Rails, will activate the Sweep Two Rails dialog. This dialog allows you to select the appropriate options and parameters required to create the new surface.

The Sweep Two Rails dialog provides two sets of parameters depending on whether you have selected the option of creating a mesh object, or any other application method for modifying an existing relief. If you select an application method for modifying a relief, the following dialog is presented.

Relief Options

Relief parameters

Application Method to modify the selected relief

Wizard prompts

If you select the mesh application method, then the proper parameters for creating a mesh object are presented in the following dialog.

Mesh Parameters

Wizard prompts

Application Method to create a mesh object

Revolutions and Extrusions Page 273

Application Method

All of the options for applying the results of the sweep two rails operation are the same as the options described in the chapter on relief creation. The options for Add, Subtract, Merge Highest, Merge Lowest, and Replace  all apply to the situation where the swept surface is to be applied to an existing relief. For this to be possible, it is necessary to select the relief to be modified before starting the Sweep Two Rails command.
The right-most application method option  allows you to create a mesh object with the Sweep Two Rails command. As shown in the dialogs above, when this option is selected, the parameters required for the command are different than when a relief is to be modified. When this option is selected, the parameters change, providing space to enter the number of slices and stacks that will make up the new object. These are described below, and the rest of the command is the same whether you are modifying a relief or creating a new mesh object.

Relief Options

These options function similar to how they work in the relief creation tool. In this case you have three options, Normal, Scale to Height, and Limit to Height.

 Normal – The new surface is created just as the selected profile and other options define it, without any vertical scaling.

 Scale to Height – The new surface is scaled to match the height parameter as it is applied to the relief. This allows you to create a surface and scale it in one step.

 Limit to Height – The new surface is limited in height by the height parameter. If a portion of the new surface extends above this height, it is truncated before it is applied to the selected relief.

Relief Parameters

The relief parameters of Height and Base are available when modifying a relief.

 Height – This value defines the height if either the ‘Scale to Height’ or ‘Limit to Height’ relief option

is selected.

 Base – This value allows you to define a base height that can be added to the extruded surface as it is applied to the selected relief.

Mesh Parameters

When the mesh option  is selected, it activates parameters that are specific to this option. They include the number of Slices and the number of Stacks that are to be used to create the mesh object.
A mesh object is composed of triangles, or facets, that make up its surface. It is necessary to instruct EnRoute regarding how many of these facets should be used to construct the object. The number of Slices is the number of sections that are used along the width of the cross sections. The Stacks value is the number of sections that are used along the rails.

Page 274 Revolutions and Extrusions

Wizard Prompts

The Sweep Two Rails tool requires more than one step in order to complete it. This portion of the dialog contains an area that contains a prompt that tells you the next step required in order to complete the function. It also contains buttons that allow you to move from step to step, back up a step, back up to the start of the function, execute the function, or exit the function.

Prompt

Buttons to change steps

The following table lists the prompts in the Sweep Two Rails tool, along with an explanation of the appropriate action.

Select the first rail

Click on the first open contour you would like to use as a rail.

Select the second rail

Click on the second open contour you would like to use as a rail.

Select the sweep sections

Click on the contours you want to use as the cross sections for the surface. EnRoute will draw a green line between the rails for each section you pick.

Following is a listing of each of the wizard buttons and its function.

Start

Return to the start of the command

Back

Go back one step

Next

Go to the next step

Execute

Execute the function

Cancel

Cancel the function

 You can use a contour more than once as a cross section. Also, remember that you can click and drag on the green lines to move the cross sections after they have been selected.

Revolutions and Extrusions Page 275

Modify a Relief

The steps in this section demonstrate how to use the Sweep Two Rails tool to modify an existing relief. In this case we will start with a flat relief in the shape of a grape leaf, and then use the Sweep Two Rails function as a way to create a more realistic surface shape for the leaf.

1. First create the 2D artwork. In this case, that includes a

contour for the shape of the leaf, contours for the cross sections, and two open contours for the

rails. The contours used for this example are shown to the right.

2. Select the leaf contour and use it to create a flat relief.

3. Select the relief, and then select Sweep Two Rails , or select the Surface menu and

then Create Surface/Sweep Two

Rails.

4. Click on Add to select that option.

5. Select the Normal application method.

 

6. Define Height = 0.00 and

Base = 0.0.

 

Page 276 Revolutions and Extrusions

7. The wizard is prompting to select the first rail. Click on the left rail contour and then click

the Next step icon in the wizard.

8. The wizard will prompt to select the second rail. Click on the right rail contour and then click Next Step in the wizard.

9. The wizard will prompt to select the cross sections. Click on the cross section contours. Each time, EnRoute will draw a green line to show where the contour was placed on the rails. The first two you identify will be placed at each end, and subsequent sections will be dividing the length.

10. You can click and drag on the green lines to move cross sections along the rails to the desired position.

 

11. Click on the Execute button to complete the command.

12. The following shows a rendered top view of the resulting relief.

Revolutions and Extrusions Page 277

This example demonstrates how the Sweep Two Rails command can be used to modify a surface to create an organic shape. In this example, with just a few more steps, the leaf surface can be completed as shown in the following image.

Create a Mesh Surface

The Sweep Two Rails tool can also be used effectively to create interesting mesh surfaces. In the following example, we create another leaf shape using a few simple contours.

 

1. Create the 2D artwork. This example requires four contours; two for the rails, and two for the cross sections. In this example, the two rail contours have been edited so that they have dimension in the z-axis rather than being flat.

 

2. Select the Sweep Two Rails  icon, or select the Surface menu and then Create Surface/Sweep Two Rails.

 

3. Click on the Mesh icon to select that option.

 

4. Define Slices = 36 and Stacks =

72.

 
 

5. The wizard is prompting to select the first rail. Click on the left rail contour and then click the Next step icon  in the wizard.

Page 278 Revolutions and Extrusions

6. The wizard will prompt to select the second rail. Click on the right rail contour and then click

the Next Step icon in the wizard.

7. The wizard will prompt to select the cross sections. Click on the cross section contours. Each time, EnRoute will draw a green line to show where the contour was placed on the rails. The first two you identify will be placed at each end, and subsequent sections will be dividing the length.

8. Click on the Execute button to complete the command.

9. The following shows a top view of the resulting object.


Revolutions and Extrusions Page 279

Page 280 Revolutions and Extrusions