The Chamfer tools allow you to modify reliefs by applying profiles that can range anywhere from a simple rounded edge all the way to an intricate profile that changes the whole relief.
Because of the way that this tool works, it is used only to modify reliefs rather than to create mesh objects. The operation of the Chamfer tools is very similar to the other relief tools.
The following image shows an example of the Chamfer Centerline tool that was used to create this intricate surface, using just one simple profile. In this case, the profile was applied to selected contours and added to the elliptical relief that already had a rounded surface.

Standard Chamfer

Menu: Surface / Chamfer / Chamfer

Toolbar: 3D Surfaces / Chamfer Centerline / Chamfer

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 that is the shape of the profile.
An analogy for this method would be to visualize the result created by passing a hand-held router with a shaper tool around the edge of a block of wood. The following image illustrates how this might look using a common bit shape.

Chamfering Page 281

Before using the Chamfer tool, this relief was a flat relief with zero height. The shape of the profile used to create the relief is shown below. This profile, which is just an open contour in EnRoute, demonstrates the general shape, with the high point on the left side and the low point on the right side that is used for most chamfer operations.

Notice that in the corners, the profile is cut off very similar to what would happen in the hand-held router analogy.
As long as the relief is wider than the chamfer profile the full width of the profile is applied. As the profile is passed around the perimeter of the relief (or the perimeter of the selected closed contours), it is possible that one side might ‘cut off’ the other side leaving only a partial profile. This can create an attractive effect, or you may see that you need to modify your profile to keep this from happening. The following graphic illustrates how this works.

Page 282 Chamfering

Step 1 – The height of the profile is added to the relief.
Step – 2 The profile is passed around one side of the relief.
The shape of the relief after Step 2.
Step – 3 The profile is passed around the other side.
The final shape of the relief. Notice that the profile was truncated where it was cut off in Step 3.
The following image shows how this looks with a relief in EnRoute.

Chamfering Page 283

Standard Chamfer Dialog

Activate the Chamfer dialog by clicking on the Chamfer icon , or by selecting the Surface menu item and then Chamfer/Chamfer. Prior to activating the command, select the relief you want edit. If you want to use separate contours to create the chamfered surface and then have this applied to the selected relief, then you also need to select these contours before activating the Chamfer dialog.

 You can edit more than one relief with a chamfer operation just by selecting all of the reliefs you want to edit before you start the command.

Chamfer Parameters

Application Method to modify the selected relief

Wizard prompts

Application Method

All of the options for applying the results of this 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 selected relief or reliefs. If you have selected contours in addition to the relief, they will be used to create the chamfer, otherwise the boundary contours of the relief will be used for the chamfer.

Chamfer Parameters

It is only necessary to specify two parameters for the chamfer command, but depending on the type of relief you are editing, your choices can have a dramatic effect on the outcome.


The Base parameter allows you to specify an additional relief height that will be added to the height of the profile contour when the chamfer is performed. The effect of this parameter is the same as with other relief creation commands.

Miter and Centerline

The Miter and Centerline specifications allow you to choose how the chamfer tool applies the profile in corners. For simple shapes and simple profile shapes, you likely won’t notice much difference, but as the shape of the relief becomes more complex, and with different profiles, this parameter becomes important.
When specifying this parameter, you have the choice of selecting Miter or Centerline, or you have the option of using neither.

Page 284 Chamfering

The best way to explain the effect of this parameter is to show a few examples. The following image demonstrates the difference between selecting Miter or No Miter using a simple rounded profile for the chamfer.

With Miter Without Miter

There are times when it may be appropriate to use a profile that does not adhere to the convention of placing the high side of the profile on the left edge of the profile. In these cases, the Centerline parameter choice will most likely be the appropriate parameter to use. The problem is that with the standard Miter option, the profile has the problem of cutting off the relief in the corners, creating a result that probably won’t be correct.
The Centerline option tells EnRoute that it is necessary to maintain an imaginary bisector of the corner angle, and not allow the profile to cut itself off as it moves into and out of the corner.
Again, an illustration provides the best illustration of this issue. In the following image, you can see that the relief on the left has the problem of getting cut off by the profile as it moves around the outside corners. Fortunately, the simple solution is to choose the Centerline option.

Miter Option Centerline Option

Chamfering Page 285

The Centerline option allows you to utilize profiles that are even more complex. The following example shows how to use a profile that replicates a raised-panel shape that is common in the cabinet-making industry.
The profile shape is shown below. The wide flat section on the left side of the profile is meant to ensure that it extends across the width of the contours.

This profile was used to create the following relief. A rounded profile was also used around the outside of the relief.

Wizard Prompts

The Chamfer tool allows you to complete the command in two steps, with the second step being options. The wizard portion of the dialog contains an area that contains a prompt for 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 to the start of the function, execute the function, or exit the function.


Buttons to change steps

Page 286 Chamfering

The following table lists the prompts in the Chamfer tool, along with an explanation of the appropriate action.

Select the chamfering contour for the shapes

Click on the open contour you want to use as the profile contour for the chamfer.

Select the chamfering contour for the holes (Optional)

Click on the contour you want to use to chamfer the holes in your relief or the holes in the selected contours. This step is optional and the profile contour selected in the first step will be used for both containers and holes by default.

Following is a listing of each of the wizard buttons and its function.


Return to the start of the command.


Go back one step.


Go to the next step.


Execute the function.


Cancel the function.

You will notice that the optional second step in the wizard is to identify a different profile contour to use for chamfering the holes in your selection. While this option will likely not be used too often, the following images show how it can be used effectively to create an interesting surface in one process.

Chamfering Page 287

Chamfer Centerline

Menu: Surface / Chamfer / Chamfer Centerline

Toolbar: 3D Surfaces / Chamfer Centerline

The Chamfer Centerline tool provides a very useful variation on the standard chamfer tool. There are two key aspects of how it works that are different from the standard Chamfer tool. First, the profile contour is extended to the center of the relief shape being chamfered; second, the profile contour is scaled as necessary to create the chamfer surface. This makes the Chamfer Centerline tool less mechanical, and allows you to create very natural-looking surfaces.
The following surface was created in one step using just the Chamfer Centerline tool.

One thing to note in this image is that EnRoute automatically adjusts the profile as the relief goes into corners, creating a very natural-looking surface. This does not require any input on the part of the user.
The following surfaces were created using the Standard Chamfer and Chamfer Centerline tools. You can see that the surface on the left provides a smooth, very pleasing surface.

Page 288 Chamfering

Standard Chamfer

Chamfer Centerline Dialog

Chamfer Centerline
The dialog for the Chamfer Centerline tool is very similar to the Standard Chamfer dialog. The wizard works identically, as well as the relief application options. The only differences are that the Relief Parameters are a little different, and you have the Relief Options that provide more relief height options. Those differences will be explained in this section. Please refer to the Standard Chamfer Dialog section for other explanations.

Relief Options

Relief parameters

Application Method to modify the selected relief

Wizard prompts

Relief Options

These options function similar to how they work in the relief creation tool. In this case you have three options, Normal, Constant Height, Scale to Height, and Limit to Height.

 Normal – The new surface is created just as the selected profile and Relief Parameters define it, without any additional vertical scaling.

Chamfering Page 289

 Constant Height – The new surface is created to match the height specified in the Height


 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.

 With the Scale to Height option, the relief is first created using the Normal option, and then it is scaled so that the maximum height of the relief matches the Height parameter.
The Constant Height option works quite well with the Chamfer Centerline tool. This is worth noting because the results you get by selecting the Constant Height option are often quite improved over the results without it. The following image demonstrates the different results that can be obtained by choosing this option.

Normal Relief Constant Height Relief

Relief Parameters

As with all the other tools, the Base parameter provides a means of adding on to the relief height to create vertical sides on the relief.
The Height parameter will be used every time the Chamfer Centerline tool is used. The following table shows how the Height parameter is used with each of the Relief Options.


Height of the tallest point in the relief.

Constant Height

Height of the relief in general.

Scale to Height

Height of the tallest point in the relief. In this case, it gives the same results as the Normal option.

Limit to Height

Maximum height of the relief.

Page 290 Chamfering

Chamfer Centerline Example

The following example shows the steps involved in creating a relief surface using the Chamfer
Centerline tool.

1. First create the 2D artwork. In this case, that includes an ellipse that is approximately 7 inches wide by 9 inches tall. The primary artwork includes some fancy 2D clipart that is commercially available. The

open contour will be the profile for the chamfer. It is a simple Bezier curve drawn in the EnRoute.

2. Select the ellipse contour and create a 100 dpi rounded relief using an angle of 30 degrees.

3. Select the relief and the clipart, and then select the Chamfer

Centerline icon , or select the Surface menu and then Chamfer/Chamfer Centerline.


4. Click on the Add icon to select that option.

5. Select the Normal application method.


6. Define Height = 0.30 and Base =



Chamfering Page 291

7. The wizard is prompting to select the chamfer profile contour.

Click on the open profile contour to select it.

8. Click on the Execute button to complete the command.

9. The following shows a rendered top view of the resulting relief.

Baroque Chamfer

Menu: Surface / Chamfer / Baroque Chamfer

Toolbar: 3D Surfaces / Chamfer Centerline / Baroque Carve Chamfer

The Baroque Carve Chamfer tool can be used to create the look of wood carving. The tool allows you to use a different profile shape for the outside and the inside of the contour.

The following example shows the steps involved in creating a relief surface using the Baroque Chamfer tool.
1. First create the 2D artwork.
In this case, that includes a
5 inch square. The primary artwork includes some
fancy 2D clipart that is commercially available.

Page 292 Chamfering

2. The open contours will be the profile for the outside and inside chamfer. It is a simple Bezier curve drawn in EnRoute.

Outside Inside contour contour

3. Select the square contour and create a 100 dpi limited height, beveled relief using an angle of 45 degrees.

4. Select the relief and the clipart, and then select the Baroque Chamfer icon.


5. Click on the Add icon to select that option.

6. Select the Limit Height

application method.


7. Define Height = 0.50 and

Base = 0.0.


8. The wizard is prompting to select the chamfer profile contour for the outside curves. Click on the

outside open contour profile to select it. Click on the forward arrow.

9. The wizard is prompting to select the chamfer profile contour for the inside curves. Click on the inside open contour profile to select it.

Chamfering Page 293

10. Click on the Execute button to complete the command.


11. The foilawing shows a rendered perspecti>le view of the resulting relief.


- --- -- -

..... •.

... •

····· .....

······ ·



Pa9> 294 Chorrtering

16. Using 3D Meshes


The 3D modeling process uses 3D surfaces to define and depict the objects in the design. There are several different ways to accomplish this. In EnRoute, reliefs are used as the method for defining and manipulating 3D surfaces that are used to create toolpaths for output.
Another common method of defining 3D objects is as 3D meshes. These objects are made up of triangles of varying sizes that define their surface. EnRoute enables you to both create and utilize 3D meshes as part of the relief design process.
As with all of the different methods for defining 3D surfaces, mesh objects have advantages and disadvantages. One clear advantage is that many common 3D modeling software packages provide the ability to export and import mesh objects. For this reason, meshes are probably the most common type of 3D objects. There are many companies that sell 3D objects of just about any type of object that you can imagine. This may be a good way to acquire an object to incorporate into your design that would otherwise be difficult and time-consuming to create.
In addition to being able to import and use 3D models, many of EnRoute’s modeling tools provide the option of creating a mesh object rather than modifying a relief. These meshes can then be positioned, rotated and scaled in order to make them just right for incorporating into a relief design.

Using 3D Meshes Page 295

Using 3D Meshes from Other Applications

EnRoute currently imports 3D mesh objects in three different formats,
 DXF – Data eXchange Format is the format created by AutoDesk® as a standard method for bringing data into and out of AutoCAD®. It has become a standard method for exchanging data between many software packages. EnRoute imports both 2D and 3D data using this format.

 3DS – This is the format used by 3D Studio®. EnRoute imports 3D files saved using this format.

 STL – STereo Lithography is a standard method created for sharing 3D mesh surface data.
EnRoute imports STL mesh objects.

 OBJ – Alias Wavefront mesh format

Creating 3D Meshes with EnRoute Tools

Within EnRoute, there are a number of ways to create 3D meshes. Most of these methods are described in detail along with the tools that provide this option. Refer to the manual sections that describe the RevolveSpinExtrude and Sweep Two Rails functions to see how to create these types of mesh objects.


Menu: Surface / Create Primitive

Toolbar: 3D Surfaces / Create Primitive Objects

The Primitives tool is used to create a range of basic 3D shapes. These shapes can be used to build more complex shapes, or they can be used as design elements in your relief. You likely won’t nee d them too often, but they can come in handy.

Page 296 Using 3D Meshes

To access the Primitives dialog, click the Primitives icon, or select the Surface menu and then click Create Primitive. The following dialog will be activated.

Primitive selection buttons Selected Primitive Parameters

Whichever primitive button is active will activate the parameters for that primitive type. The parameters are similar between primitive types, but they are specific to that type.
The following table lists the different parameter types, along with an explanation of what that parameter defines.

X, Y and Z

These are the coordinates for the location of the center of the primitive.


This is the number of sections either around the circumference of the object or along one axis.


This is the number of sections along one axis, typically the z-axis, of the object.


This is half the diameter of a circular dimension of the object.


This is the z dimension of the object.


This is the dimension along one axis of the object, such as

‘X Size’.

Sweep Angle

For the Torus object, this is the number of degrees of the

sweep of the object around the ‘outer’ radius.

Close top or Close Bottom

You can choose whether Cylinders, Cones and Boxes should have surfaces that cover their tops and bottoms.

Using 3D Meshes Page 297

Slicing Meshes

Menu: Surface / Apply Mesh

Toolbar: 3D Surfaces / Apply Mesh to Relief

This tool allows you to apply slices to a mesh with the option of using the X, Y or Z axis.

Slice Meshes Dialog

After selecting a mesh click on the Slice Mesh icon, or select the Surface menu and Slice

Meshes to activate the dialog.


Slices will be created in the Z axis. Horizontal slices created from bottom to top.


Slices will be created in the X axis. Vertical slices created in the front view.


Slice will be created in the Y axis. Vertical slice created in the right view.


This is the thickness of the slice. This is usually the thickness of the material that is being used for the project.


The number of slices is calculated based on the thickness defined, and on the dimension of the model along the active axis.


This parameter is the distance from the bottom of the plate that the first slice is calculated. Most often this would be set at 0.00, but you can also move the bottom slice up if that fits the model better.


Check this box to create the separate slice geometry that will be used to create toolpaths.


Check this box to label the separate layer pieces.


This create a model to show how the layers will look once they are assembled.

Page 298 Using 3D Meshes

Slice Mesh Example

The following example shows the steps involved in slicing a simple mesh.

1. First create or import the mesh. Select the mesh. In this example the mesh measures

6x6x5 inches.

2. Click on the Slice Mesh icon, or select the Surface menu and then Slice Meshes to activate the dialog.

3. Enter the parameters:

Select the Z Axis (This is the one you will likely use the majority of the time)

The thickness of the material in our case is.5 inches. The program calculates the number of slices to be 10.

We did not want any offset from the bottom of the plate, so this parameter is 0.00

Check the Layout, Label and Model parameters.

4. This is a 4 view preview of the parameters using the Z axis selection.

Using 3D Meshes Page 299

5. Click on the Apply button to create the slices.

6. This is the top view: The layout shows

each of the layers as a

separate item to the right of the mesh and the model of the

assembled product is placed to the left of thee mesh.

This image shows the preview of this example if the X axis had been selected.

Page 300 Using 3D Meshes

This is the results of selecting the X axis. You can see that the axis choice will change the shape and assembly method of the model.

This image shows the preview of this example if the Y axis had been selected.

Using 3D Meshes Page 301

This is the results of selecting the Y axis.

Page 302 Using 3D Meshes

The following images show how a more detailed model can provide interesting results by using mesh slicing to create a stacked version of the model.

This is a screen shot showing the original model along with a model of the slices created with the slicing tool.

This is a photograph of the stacked model that was made by cutting slices
using ¼” thick plywood.

Using 3D Meshes Page 303

Applying Meshes to a Relief

Menu: Surface / Apply Mesh

Toolbar: 3D Surfaces / Apply Mesh to Relief

After meshes are created or imported, their primary function is to be used to modify relief surfaces. The Apply Mesh  tool is used to accomplish this.
In order to enable the Apply Mesh function, it is necessary to have at least one relief and one mesh in your selection. After selecting a mesh and a relief, click on the Apply Mesh icon , or select the Surface menu and Apply Mesh to activate the dialog. To complete the function, just click on the Apply button.

Apply Mesh Dialog

Selector between Faceted and Smooth option

Smoothing level for smooth option

Application Method to modify the selected relief

Faceted or Smooth

One of the characteristics of a mesh surface is that it is composed of triangles, or facets, that make up its surface. When a mesh object is applied to a relief surface, the facets can be quite obvious and may be an undesirable characteristic.
EnRoute provides a Smooth  option that implements a means of smoothing out the facets of the mesh to provide a smoother finished surface. For surfaces that are intended to be smooth, the results of using this option can be quite dramatic. If the Faceted  option is selected, then the object is applied to the relief surface using its facets directly.
The following images show the difference that can be realized by using the Smooth option.

Page 304 Using 3D Meshes

Application Method

All of the options for applying the results of this operation are the same as the options described in the chapter on relief creation. The options for AddSubtractMerge HighestMerge Lowest, and Replace  all apply to the selected relief or reliefs.
The vertical location of the mesh relative to the vertical location of the relief controls how much the relief is modified. It is important to position the mesh object correctly in the z axis relative to the relief, so when it is applied to the relief, the results are correct.
The following image shows a front view that includes a relief and four mesh spheres that are located at different positions in the z axis. A perspective view of the relief shows the results of applying these objects to the relief using the Add option.

Using 3D Meshes Page 305

Relief surface

Front View showing vertical position of meshes and relief

Perspective view of the relief after meshes were added

Using a Mask

There may be times when it is desirable to use just a portion of a mesh object in your design. This can be accomplished by using a mask. A mask is just a closed contour that is selected along with the relief and the mesh object when the Apply Mesh command is started.

Page 306 Using 3D Meshes

The following image shows a large relief, 3D mesh of a lion, and a smaller elliptical contour which acts as the mask. All three of these elements are part of the selection.

With these selected, execute the Apply Mesh command to add the mesh to the relief. The result is shown in the next image.

Using 3D Meshes Page 307

After adding some borders to the relief to complete the design, you see a perspective view of the relief in the next image. You can see how the use of the mask made it simple to incorporate only the portion of the mesh object that was needed.

Page 308 Using 3D Meshes

Unwrapping Meshes for Rotary Axis Support

Menu: Surface / Unwrap Mesh

Toolbar: 3D Surfaces / Unwrap Mesh onto Relief

EnRoute provides support for rotary axis cutting with the ability to wrap designs when they are output. At first this can seem like an intimidating task, but virtually all of the design can be accomplished in the very same way you would design for normal cutting on a router. The thickness of the plate represents the Radius of the rotary cylinder, and then typically the height of the plate corresponds to Circumference of the rotary cylinder.
3D Mesh objects are also supported, with the ability to add them to a relief in such a way that they can be wrapped onto the cut cylinder when they are output providing the ability to cut full models very effectively. The advantage of this approach is that, once again, all of the design work can be accomplished without having to change the design environment you are already familiar with.

Here are a few images of models that have been cut using EnRoute’s unwrapping tool.

Using 3D Meshes Page 309

The first step is to import a mesh object and to then orient it correctly relative to the relief surface. The following image shows a model that was used to cut a replica of the Michelangelo’s David sculpture. This is a very nice model that was purchased for this use.

The following steps list the process of setting up the job to cut this model 6” diameter material.

Page 310 Using 3D Meshes

1. First, we know that we need to mill a 10” diameter cylinder from a rectangular block of material

that is 10” x 10”. This means that we will “turn” the rectangle down to a uniform 10” cylinder.

When it turns, we need to first take into account the diagonal dimension of the rectangular material. In order to do this, define a material thickness of

14.142 / 2 = 7.071.

2. Now, with the machine we are using, we want to set the Plate definition at Bottom of Plate and simply draw a line along the X axis. An engraving toolpath will move the tool along the rotary axis in order to allow us to “turn” our material down to the correct diameter of 10” (5” radius).

A depth of 2.071” in 3 passes

seems appropriate.

Our machine rotates at 30 rpm for cutting. With a ½” diameter tool, this corresponds to approximately 15 inches per minute for a feed rate along the axis.

3. The engrave toolpath is sent to the machine, and output is configured to allow the machine

to operate in “lathe” mode for this

type of cutting.


Using 3D Meshes Page 311

4. Now we are ready to set up the design to unwrap the model onto a relief and then toolpath it to get it ready for cutting.

Set the thickness of the plate at


Check the Wrap Plate option and select Wrap X Axis. This will automatically set the Height of

the plate to match the circumference of the cylinder.

Set the length of the plate at 18”

5. Most of the work will be done with the Plate unwrapped for design purposes. This can be toggled using Control+Shift+X to toggle between wrapped and unwrapped mode.


6. Import the mesh model and position it along the X axis, and centered at the X axis.

Page 312 Using 3D Meshes

7. Now create a flat relief that is the same size as the plate.

8. Select both of these objects and then select the Unwrap Mesh tool . It is located in the Surface menu, and is also located on the

3D Surfaces toolbar as a flyout with the Mesh Slicing tool.

9. It is only enabled if you have both the mesh and relief selected. As soon as you activate the tool it gets to work on unwrapping the mesh onto the relief

10. The result of the unwrapping process is always interesting.

Using 3D Meshes Page 313

11. When the plate is wrapped, you see that the relief wraps back to create the model, as expected. This surface can now be toolpathed just like you would any other unwrapped relief. When the toolpaths are output to the machine, instructions for properly wrapping them back onto the rotary axis allow you to achieve success.

Page 314 Using 3D Meshes

17.Modifying and Combining Reliefs


After you have created a relief, EnRoute provides many tools that allow you to modify it to fit the needs of your design. This chapter provides descriptions of the tools that are available for modifying reliefs as part of your design process.

Selecting Reliefs

To select a relief, click on the contour that defines its perimeter.
You can also select multiple reliefs using one of the following methods:
 Hold down the SHIFT key and click on the reliefs one after the other.

 Click and drag to draw a selection box around the reliefs.

Cutting, Copying and Pasting Reliefs

One handy aspect of reliefs in EnRoute is that they exist in the same workspace as all of the other EnRoute object types. This means that they can be treated in much the same way as any other EnRoute object.

Cutting and Pasting

To cut and paste reliefs:
1. Select the reliefs to cut.
2. From the Edit menu choose Cut, click on the Cut Iconor press Ctrl+X.
3. Select the drawing where the reliefs are to be pasted.
4. From the Edit menu choose Paste, click on the Paste Icon, or press Ctrl+V.

 After a relief is placed on the clipboard either by cutting or copying it, it remains there until it is replaced by something else. This allows you to paste it more than once.

Modifying and Combining Reliefs Page 315

Copying and Pasting

To copy and paste reliefs:
1. Select the reliefs to copy.
2. From the Edit menu choose Copy, click on the Copy Icon or press Ctrl+C.
3. Select the drawing where the reliefs are to be pasted.
4. From the Edit menu choose Paste, click on the Paste Iconor press Ctrl+V.

 Another easy way to copy a relief is to click and drag on it while pressing the CTRL key. When you release the mouse button a copy of the selected reliefs is placed at the new location.

Deleting Relief Objects

To delete one or more reliefs:
1. Select the reliefs.
2. From the Edit menu, select Deleteor you may also just press the DELETE key.

 Deleting relief objects is the same as deleting any other object in EnRoute.

Clearing Reliefs

Clearing a relief removes the relief surface from the object, but it retains the contours that made up the perimeter of the relief. You will use this during the relief design process to clear a relief so that you can recreate it using different parameters.
To clear a relief:
1. Select the relief.
2. From the Surface menu, select Delete Relief, or just select the Delete Relief Icon  from the relief toolbar.

Page 316 Modifying and Combining Reliefs

Moving Reliefs

Moving reliefs is done much the same way as moving any other object in EnRoute. You can click and drag on a relief object to move it in the top, front and right views.
The key difference is that the vertical position of a relief object is very important when it comes time to create toolpaths and output toolpaths. In addition to the Precision Input Center, EnRoute provides several tools to help you position relief objects in the z-axis.
To move a relief using the Precision Input Center:
1. Select the relief in the view (Top, Front or Right) that you want to use as the reference plane.
For example, in the Top view the reference plane is the X-Y plane. In the Z axis this plane is located at the closest Z-location on the object(s) you have selected.
2. Press F2 to activate the Precision Input Center.
3. Click on the Move tab.
4. Click on the button that represents the corner of the object you want to specify.

5. Specify the X, Y, and Z coordinates for the selected corner.
6. Click on the OK button to finish moving the object(s).

Vertical Positioning of Reliefs

The method for positioning reliefs described above works well, and you can use this method exclusively; however, EnRoute also provides tools that are specifically designed to assist you with positioning reliefs vertically within the boundaries of the Plate.
Access the Align Reliefs tools by clicking on the Align Relief icon in the Relief toolbar to activate the
Align Reliefs flyout toolbar.

The following table describes the function of each of the Align Reliefs functions

Align reliefs to bottom of plate

Aligns each of the selected reliefs to the bottom of the plate.

Align selection 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 reliefs to top of plate

Aligns each of the selected reliefs to the top of the plate.

Modifying and Combining Reliefs Page 317

Align selection 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 reliefs to middle of plate

Aligns each of the selected reliefs to the middle of the plate.

Align selection to middle 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 bottoms to top of plate

Aligns the contours for the relief to the top of the plate. This is the default location for contours and reliefs, and it often works best when modifying reliefs to have it located at this default location.

Rotating Reliefs

Rotating reliefs is accomplished the same way as rotating any other objects in EnRoute. Refer to the section on Rotating Contours in the Arranging Contours chapter.

Page 318 Modifying and Combining Reliefs

Scaling Reliefs

Scaling reliefs is accomplished the same way as scaling any other objects in EnRoute. You can either scale the relief by selecting it and then clicking and dragging on one corner of the selection box, or you can use the Precision Input Center to precisely scale the relief. (See the Scaling Contours description in the Arranging Contours chapter)
When it comes to scaling reliefs, there is an important consideration involving the resolution of the relief. Remember that when you first create a relief, you specify a resolution for that relief. This specifies the resolution of the grid that defines the relief surface. After the relief is created, the total numbers of grid points that define the relief are set. So, if you scale the relief, the effective size of the grid points in the relief is scaled too.
If you created a relief that was 50 mm x 50 mm with a resolution of 100 dpi and then scaled it up to a size of 500 mm x 500 mm, the effective resolution of the relief would drop to 10 dpi. This illustrates that it is important to consider the effect of scaling a relief, and the effect that it will have on the quality of the finished piece.
The following image shows how the size and shape of the relief grid is affected by a scaling operation.

Original Relief Scaled Relief

Modifying and Combining Reliefs Page 319

Fit Relief to Plate

Menu: Surface / Fit to Plate

Toolbar: 3D Surfaces / Modify Relief / Fit to Plate

You can use the moving and scaling tools in EnRoute to size and position a relief just as you would other objects. There are times, however, when it would be useful to be able to automatically fit a relief into your plate as you get it ready for toolpaths. The Fit Relief to Plate  function provides this capability. It will automatically position and scale a relief so that it fits vertically within the defined plate in your active drawing.
To fit a relief to the plate:
1. Select the relief.
2. From the Surface menu, select Fit Relief to Plate.

Smoothing Reliefs

Menu: Surface / Smooth Relief

Toolbar: 3D Surfaces / Modify Relief / Smooth Relief

There are times when you are working on a relief design when it will be useful 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. EnRoute provides the Smooth Relief  tool accomplish this.
1. Select the reliefs to be smoothed.
2. From the Surface menu, select Smooth Relief.
3. Click and drag to set the Smoothing Radius and Smoothing Power.
4. Click Apply.

 You can apply the smoothing function to a relief more than one time in order to smooth it more and more.

The following image shows an example of the results of smoothing a relief.

Page 320 Modifying and Combining Reliefs

Smoothed Relief

 You can apply smoothing to just a portion of a relief by selecting a contour along with the relief.

The selected contour(s) acts as a mask, and the relief will only be smoothed within the boundary
of the contour.

Inverting Reliefs

Menu: Surface / Invert Relief

Toolbar: 3D Surfaces / Modify Relief / Invert Relief

Inverting a relief has the effect of reversing the z-coordinates of the relief relative to the location of the
perimeter contours of the relief. This is a simple way to convert a ‘positive’ relief to a ‘negative’ relief.

To invert a relief:
1. Select the reliefs to be inverted.
2. From the Surface menu, select Invert Relief
You can also select the Invert Relief function from a screen icon. The function is located on a flyout toolbar that is activated by clicking a holding the Smooth Relief icon. The flyout is shown to the right.
One thing you can see in the images above is that inverting a relief only modifies it in the z axis. If you plan to invert a relief to use it as a mold, it may also be desirable to mirror the relief prior so that any impressions created from a mold have the proper x-y orientation. A relief can be mirrored using the same method as any other EnRoute object. From the Transform menu, select Mirror and then either Mirror Horizontal or Mirror Vertical.

Modifying and Combining Reliefs Page 321

The following images show the sequence of actions to both invert and mirror a relief in preparation for using it as a mold.

Page 322 Modifying and Combining Reliefs

Adding a Draft Angle to a Relief

Menu: Surface / Apply Draft Angle to Relief

Toolbar: 3D Surfaces / Modify Relief/ Add Draft Angle

When you create a relief, you will often create portions of the relief that have a vertical side. This vertical side can be problematic for two reasons. First, if the vertical side is relatively tall, its height could be greater than the cutting length of the tool you will use to mill it with. This can cause problems that might cause the tool to break. Second, if you are going to use the finished piece to create a mold you may need to provide a draft angle in order to allow the molded pieces to come out of the mold properly.
EnRoute provides a Draft Angle  function that allows you to add a draft angle to your relief.

To add a draft angle:


Select the relief.



From the Surface menu, select Apply Draft Angle.

You can also access the tool

through the Modify Relief Toolbar.
3. In the Precision Input dialog, enter desired values for Draft Angle and Height Threshold. (The draft angle is usually between 3 and 7 and the Height Threshold refers to the starting point of the angle.)
4. Click Apply.

Modifying and Combining Reliefs Page 323

Create a mesh surface from a Relief

Menu: Surface / Create mesh surface from relief

Toolbar: 3D Surfaces / Modify Relief / Create a mesh surface from relief

This tool allows you to create a mesh from an existing relief.

1. Select the relief.


2. Click and hold the Smooth icon, then click on the Create mesh from relief icon.

Smooth Icon Create Mesh from Relief

3. Enter the Mesh tolerance in the parameters field and click Apply.

4. The mesh will be created and placed in the same location as the relief.

Relief Relief and Mesh Mesh

Page 324 Modifying and Combining Reliefs

This is an image of a relief that was created in order to create a mesh from it.

Here is a rendered image of the resultant mesh object. Mostly what you notice is how precisely the mesh replicates the original relief.

Here is a close-up of the un-rendered mesh. Notice how the facet density is adjusted as necessary to get detail.

Modifying and Combining Reliefs Page 325

Offset Relief Surface

Menu: Surface / Offset relief

Toolbar: 3D Surfaces / Modify 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.

1. Select the relief.
2. Click on the Offset Relief Surface icon.  This can be found in the 3D Surfaces toolbar in the Modify Relief flyout toolbar. It is also in the Surface Menu.
3. This will open the Offset Amount dialog.

4. Enter the amount that you wish to offset the relief surface.
5. Click Ok. This will apply the offset to the surface of the relief.
The following images shows a relief before and then after the offset was applied.

Page 326 Modifying and Combining Reliefs

Merge Reliefs

Menu: Surface / Merge Reliefs

Toolbar: 3D Surfaces / 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.
The following graphic shows the dialog that is activated when you select the Merge Reliefs 

Wizard Prompts

Application Method to modify the selected relief

As you can see, it is not a complicated dialog. To complete the merge action, it is just necessary to select the application method for how the reliefs will be merged, select the base relief and then select the relief(s) that will be merged with the base relief.
The following example illustrates the process.

1. First create the reliefs that you will merge. In this case we have created two simple reliefs, an ellipse and a star.

2. Position the reliefs correctly for merging.

Modifying and Combining Reliefs Page 327

3. Select Merge Reliefs


4. Click on the Add icon to select that option in the dialog.

5. The wizard prompts you to select the base relief. Click on the ellipse relief to select it, and then click on the Next  button.

6. The wizard prompts you to select the reliefs to merge. Click on the star relief to select it, and then click on the Execute button to complete the merge.

7. This image shows the result of the merge action.

This image shows the merged relief along with the original star relief.

 The Merge Relief tool can merge reliefs of different resolutions, and reliefs that have been rotated and scaled without any problems.

Page 328 Modifying and Combining Reliefs

Combine Reliefs

Menu: Surface / Combine Reliefs

Toolbar: 3D Surfaces / Merge Reliefs / Combine Reliefs

Use the Combine Reliefs tool to combine one or more selected reliefs.

The example below demonstrates three separate reliefs combined into one relief in two different ways.


Select the reliefs to be combined.



Click and hold the Merge Reliefs Icon

to open the flyout toolbar.


Click on the Combine Reliefs Icon.


 If the reliefs overlap they will combine to create one relief with one contour.

 If one of the reliefs is completely enclosed within another, it will create a hole in the relief.

Extract Relief Slices

Menu: Surface / Extract Slices

Toolbar: 3D Surfaces / Merge Reliefs / Extract Slices

The Extract Slices tool allows you to “cut” the relief into layers. Use this tool to “stack” your material to create large objects. For example, if your material is 1.5 inches and the object that you want to create is 4 inches, you can cut your relief into 3 slices and then stack the material to create the object.
EnRoute now includes the ability to also create contours with each slice that represent a mask for creating toolpaths. Most of the slices you create will include a flat area that corresponds to the top of the material. It typically isn’t necessary to create toolpaths for this part of the relief. The masking contours make it very easy to create toolpaths only for the portion of the slice that is part of the finished relief surface.

Modifying and Combining Reliefs Page 329

Extract Slices Dialog


Slice Thickness

The thickness of each slice. This is typically the actual thickness of the material you are cutting.

Slice Count

The number of slices that you want to create.

Slice Bottom

Typically, the bottom of the relief, but it is also sometimes handy to move the bottom of the bottom slice up a little so that any flat background can be removed.

Produce Mask

Should the masking contours be created.

Mask Offset

Offset from the edge of the slice edge and the edge of the flat areas. This

provides some room for the toolpaths to “overcut” the slice.

Separate Layers

Check this parameter if you want to create new layers for each slice.


Click to create slices.


Click to close the tool.

This example is showing how this design was extracted from the background relief.

1. Click and hold the Merge Relief iconto open the flyout toolbar then click on the Slices icon.  This will open the Slices Dialog.

2. Click on Front to work in the front view and then click on the relief. The relief information is loaded into the Slices Dialog.

Page 330 Modifying and Combining Reliefs

3. In this example, we created 6 slices with a thickness of 1.5. The bottom of the slice is located .02 from the bottom of the relief.
4. As you change the parameters you will notice that the pink lines represent the slice position.
5. Click on the Apply button.
6. The slices will be created separately on different layers when the Separate Layers parameter has been checked.
This is slice layer 1.
You will notice that since we defined a Bottom of the first slice as begin slightly above the bottom of the relief, the flat background from the original relief is gone.
7. This shows all 6 slices separated to make them easier to tell apart. What’s left now is to move each of them down into the plate so
that toolpaths can be created, and then fit them on the
material for cutting.

Modifying and Combining Reliefs Page 331

8. This shows a portion of one of the slices, highlighting the mask contours that were created to make it easier to create toolpaths only where needed.

Page 332 Modifying and Combining Reliefs

18.Using Bitmaps


EnRoute utilizes bitmap images as a method for modifying relief surfaces. Bitmaps can be useful in creating a texture that makes up part of your design. They can also be useful as an efficient method for getting design information into EnRoute that might be difficult to create using other methods.
EnRoute utilizes the colors or grayscale shading in a bitmap image to modify the height of the relief using parameters that you provide. The process of applying a bitmap to a relief is simple, but it can be used in many different ways to create intricate surfaces.

Applying Bitmaps to a Relief

The following graphic shows the dialog that is activated by the Apply Bitmap  tool. This function is activated by Selecting Surface/Apply Bitmap, or by selecting the Apply Bitmap  icon from the 3D Surfaces toolbar.

 Height of the applied bitmap

Application Method to modify the selected relief

Using Bitmaps Page 333

The Application Method defines how the bitmap will be applied to the relief surface. Typically, you will select either the Add  or Subtract  method in order to apply either a positive or negative version of the bitmap. The Height parameter defines the maximum height of the bitmap as it is applied.
The following simple example illustrates the process of applying a bitmap to a relief.

1. First create the relief that you want to add the bitmap to, and also import the bitmap file into your drawing. In this case, we have created an ellipse as the relief, and have imported a bitmap of a brick wall that will be used as a texture.

2. Position the bitmap on top of the relief.

3. With both the relief and the bitmap selected, choose the Apply Bitmap tool by selecting Surface/Apply bitmap .


4. Choose the Application Method and the Height. In this case, choose Add, and define a Height of 0.20.

5. Click Apply.


6. This image shows a rendered perspective view of the results.

Page 334 Using Bitmaps

Using a Mask

When you apply a bitmap to a relief, you may not always want to apply the bitmap to the entire relief. EnRoute provides a method for masking the bitmap so that it applies only to the desired portion of the relief.
Any contour that is not part of the relief boundary or that does not have toolpaths applied to it can be used as a mask. It is only necessary to select the masking contours along with the relief and the bitmap when you activate the Apply Bitmap function. You will notice that the masking contours are automatically sorted into groups of containers and holes, and when the bitmap is applied only the portion of the bitmap that is inside the mask will be applied.
The following image shows a relief that had a bitmap texture applied using letters as a mask.

Using Bitmaps Page 335

3D Effects using Bitmaps

It is possible to create realistic 3D effects using bitmaps, but this requires bitmap images that are created with this in mind. Remember that when a bitmap is applied, the colors and shading in the image are what control how the bitmap modifies the relief.
In a grayscale image, the different shades of gray on the scale from white to black define the height of the bitmap. The Height parameter that you define provides the overall height of the bitmap. With a grayscale image, white colors would be applied at this Height value, and then the shades of gray would be shorter down to black which has no effect on the relief.
The following image shows an example of a grayscale drawing that was created in order to have the proper effect on a relief.

You can see that the lightest shades in the waves will be the tallest parts of the bitmap. Since the fish
is a little darker, it will be less tall, and the background is black so it won’t affect the relief.

Page 336 Using Bitmaps

The next image shows a relief after this bitmap has been applied. You can see that the shading provides a finished relief that is quite realistic.

The next thought you may have is that it would be nice to be able to apply a photograph to a relief to get a 3D effect. It certainly is quite feasible to use a photographic image in a relief. Remember thought that EnRoute uses the shading in the image to determine height. Something that is taller in the photograph may or may not be a lighter shade than objects that are further back in the image. Since a photograph is flat, it does not provide 3D information to the software to determine realistic heights.

Using Bitmaps Page 337

The result you get with a photograph may or may not be what is desired for the subjects in the photograph. The following images show a photograph, and the relief surface that was created using the image.

Page 338 Using Bitmaps

19.Texture Tools


As discussed in the previous chapter, it is useful to utilize bitmaps to add textures to relief surfaces; however, bitmaps present some challenges too. You are dependent on the size and resolution of bitmaps, and regardless of how bit they are, there are limits to their size and scalability.
EnRoute contains several other great options that provide a way to create interesting textured surfaces that don’t rely on the use of bitmaps. Parametric Textures provide a limitless way to create surface textures for your designs. EnRoute contains 19 unique parametric textures, and each one of them can be modified endlessly to create surfaces. Some of the things that are special about parametric textures include,

 Parametric textures are continuous, extending endlessly in all directions.

 Parametric textures are three dimensional. This means that you get different results when you apply them to surfaces with a shape, as opposed to applying a texture to a flat surface.

 Parametric textures are completely scalable in all directions. You can stretch them in any axis in order to change the look entirely.

 Templates let you get back to exactly the same results you got last time without having to keep track of separate files.

 You really can create your own effects and then keep them to yourself or share them with others.

 Parametric textures can be combined to get even more unique results.

 Parametric textures automatically have exactly the same resolution as your relief.

Texture Tools Page 339

One of the limitations of using textured relief surfaces is that as the relief becomes larger, the time it takes to mill the relief surface can become lengthy. When you create toolpaths to mill the surface, you typically define a large overlap of the fill toolpaths in order to minimize the visibility of the tooling marks. Another texturing option is called Rapid Texture, and this method takes a different approach. Rapid Texture uses the size and shape of the tool as one of the design elements of the texture. This allows the use of larger ball end mill, conic, and end mill tool to create a surface texture, and it provides a method for creating very interesting surfaces that can be milled quickly and efficiently.

This chapter explains Parametric TexturesRapid Textures, and a specialty use of Rapid Texture that we call Rapid Picture.

Page 340 Texture Tools

Parametric Textures

Menu: Surface / Textures

Toolbar: 3D Surfaces / Textures

EnRoute offers 19 separate parametric textures. The following table provides a brief overview of each texture.


Replicates the look of a bamboo panel.

Basic Noise

This is the basic noise algorithm that is the basis for all of the other parametric textures.


This gives lots of options for creating a brick pattern that varies from smooth and uniform to rough and jittery.

Texture Tools Page 341


This is a great texture for adding a hand-tooled effect on virtually any surface. The size and shape of the “cells” can be varied to give just the right amount of roughness.


Get anything from uniform sized and spaced half spheres, to a rough and distorted dinosaur skin texture.


A nice replication of a stone surface that can be rough or smooth.


Add some fire to your design with a texture that evokes

the feel of dancing flames.

Page 342 Texture Tools

Flow This is a gorgeous texture that evokes the elegant flow of water. It offers endless possibilities.

Hammered This texture lets you replicate the look of hammered metal, controlling the size, roughness, and visibility of the cells. Great as a background texture.

Hexes Anything from a uniform hexagonal pattern to a rough and distorted surface. This example shows something

in between.

Marble A texture that evokes the swirling pattern in a marble slab.

Texture Tools Page 343


Fun, bizarre, cool. When you first see the Mudpot texture, you know that you have to use it on a design. It’s the closest you will come to psychedelic in EnRoute.


This is a versatile texture that can add interest to any surface you apply it to. As with most of the parametric textures, this is a 3D texture, so you get different results if you apply it to a relief that has a 3D shape to it rather than just a flat relief.


Another versatile texture that can take on lots of different looks, depending on how gritty or smooth you would like it.


Another elegant, flowing texture. This one is different than flow in that elements of the texture can come to sharp peaks. It’s great for architectural uses.

Page 344 Texture Tools


This texture may be the

most fun to experiment with. You really can create

textures that look like a

terrain surface. Larger surface elements interact

with a whirling surface.


A wood texture that lets you specify the size of the veneer panel. This allows you to have a pattern that gives the appearance of a matched veneer panel.


A tight, uniform weave, to a loose wavy weave. Smooth strands or rough. Weave textures are cool, and you can get just about any type

of weave you desire with this texture.


Realistic or exaggerated, you can essentially position the log and then determine how you are going to cut through it. This is a fun texture to use to get a great wood texture for your piece.

Texture Tools Page 345

Following are some examples of selecting and applying a Parametric Texture. The basic steps include,

 Create a relief surface to which you want to add the texture.

 Select the relief.

 Choose the texture you want to use from the texture flyout toolbar.

 Define the parameters for the texture, using the preview as a guide.

 Choose the application method – add, subtract, merge high, merge low, replace.

 Define the height of the texture.

 Click Apply.

Texture Dialog

The left section of the textures dialog includes the same information for all of the texture types. The right section of the dialog contains parameters specific to each type of texture. The dialog is used in the same manner for each of the different textures. The first section of the dialog is described below:

This icon allows you to get specific information about the texture type that you have chosen. The name of the Texture is listed here and you can click on the information icon  to get specific information for each of the parameter settings.

This section works the same way as the create relief section. Add, Subtract, Merge Highest, Merge Lowest, and Replace. See the create reliefs section for more information about these parameters.


Height specifies the overall height of the texture that will be applied.

Page 346 Texture Tools


The template section is used to create and store specific design parameters so that they can be easily brought back later.

EnRoute includes a selection of templates that provide a good starting point for creating textures.

Click on a template to load its parameters.


You can also create your own specific texture designs and name and save them to the template library.

Once the new parameters have been entered; Click on the Save button.

Enter the name of the template that you wish to save and click OK.


If you choose to delete a template, click on the name of the template that you want to delete and click the delete button. A dialog will open asking you to confirm that you want to delete this template.

This section shows you a small preview of the parameters that you have entered. It is a nice tool to use while you are designing and creating new textures for your designs. The preview is updated whenever you change a parameter value, and it is based on the actual size of the selected relief.


Press Apply to apply the texture to the selected relief.


Click Close to close the Texture Dialog without applying a texture.


Reset will change the parameters back to the default parameters for the specific texture.

Texture Tools Page 347

Parameters Section of the Textures Dialog

Each of the Texture types has its own set of parameters. The example below is the dialog for the bricks texture.

Click on the information icon  to get information about the texture. Scale and Position are available for each texture. Scaling the texture differently in the X and Y directions is a good way to stretch the texture to get different results. Textures aren’t limited in size, but the position lets you control how the texture will be applied to your selected relief. This is usually used to fine tune your results. All of the other parameters are specific to your selected texture. Things like Power, Jitter, Twist, and Roughness are all ways to make a texture more or less uniform, smoother or rougher – it’s how you make your texture fit your needs. Feel free to try things out and be creative, that’s the fun part.

Example using the Brick Texture:

1. In this example, the brick texture is shown on 4 different shapes of reliefs. Flat, Rounded, Beveled and Limited
Height. Create simple a simple
ellipse shape and
then make some copies.
2. Create some different relief

Page 348 Texture Tools

3. Select the reliefs and click and hold the Textures icon in the 3D Surfaces Toolbar. This will activate the flyout menu.

4. Click on the Brick

Texture Icon.

This will open the

Precision Toolbar.

 EnRoute saves the last texture that was used as the icon in the 3D Surfaces Toolbar. For example, if the last texture you used was the Brick Texture, then the brick icon would be the one in the 3D Surfaces toolbar and you would only need to click on the icon to activate the Brick Precision Toolbar. This helps to streamline the creative process.

5. Select the Parameter: Add to Relief.

6. In this example we simply chose the “bricks” template from the template section.

Click on the arrow to open the drop down list. As you highlight the choices in the list, the preview window will show you a small example of the texture.

 You can, of course, also choose to create your own new texture by adjusting the parameters. The Information icon provides you specifics about each parameter and the preview window allows you to see the changes as you develop the new texture.

7. Click on the Apply button to apply the texture to the reliefs.

The textures will be applied to the reliefs and the

Texture Tools Page 349

Precision Toolbar will close.

 Notice how the texture is consistently applied to each of the different shapes.

 Signs can be easily created using the textures with masks.

Page 350 Texture Tools

Symmetric Parametric Textures

Parametric textures are a very interesting and flexible method for creating surface textures in EnRoute. Textures can be applied to almost any surface to make them more interesting. EnRoute now includes a new set of textures that are automatically symmetric.
This is an example of the Phase 2 texture

They are very similar to the standard parametric textures on which they are based, except that pattern is more tied to the size of the panel you are creating, along with specifiers for the ‘density’ of the pattern
– these parameters are called WavesX and WavesY. You can see that as these parameters are increased, the texture becomes denser in whichever direction you are changing. The Waves parameters allow the texture to be calculated so that it repeats both top to bottom and left to right.

Texture Tools Page 351

The following image is the same texture from above, copied so that it repeats four times. You can see that it matches perfectly from left to right and from top to bottom. This capability allows you to create panels that can be reproduced either by milling them multiple times, or by using a molding and casting method, that allows the pattern to be repeated on a larger scale.

Rapid Texture

Rapid Texture is based on an interesting concept. Rather than working to limit the impact of the shape and size of the cutting tool, embrace the tool as a design element and create “toolpath” that use the shape and size of the tool as part of creating an interesting surface texture. This approach introduces some interesting characteristics.

 It typically isn’t necessary to do much, if any, surface preparation after cutting and prior to applying a finish. There aren’t tooling marks that you are trying to remove.

 The number of toolpaths required to get achieve the surface is greatly reduced from milling a

3D surface. This means that the time to produce the finished surface can be dramatically reduced.

 Even though you are reducing the machine time, you add perceived value to your end product.

 The range of surface texture that can be achieved with this one approach is pretty amazing.

 You tend to use larger cutting tools. This limits the amount of detail that can be achieved, the

Rapid Texture is still very versatile. Incorporating 3D surfaces is still quite feasible.

Page 352 Texture Tools

This is an example of Rapid Texture using a 90-degree Conic tool.

What’s a Seed Contour

Rapid Texture is created by creating offset contours and then distorting them using EnRoute’s unique noise algorithms to create an interesting pattern. In order to be able to create an offset, it is necessary to have a starting point, and this is what we refer to as a Seed Contour. It’s the starting point that EnRoute uses for offsetting.
What’s cool about the seed contour concept is that it provides a great way to add to the interest of the texture. You can select one contour or several. They can be open or closed. Seed Contours are part of the creative design process with Rapid Texture.

 In EnRoute 6, it is now possible to create a Rapid Texture pattern without having to select a contour to serve as the seed contour. In this case, EnRoute will automatically create the required seed contour for you. It will be a straight line across the limits of the texture. For many uses, this might be fine, but the ability to use your own seed contours is not limited.

Texture Tools Page 353

This is a typical open contour seed contour

Here are the results of rapid texture using this seed contour.

Basic Steps Rapid Texture

1. Create and select a seed contour, if desired.
2. Click on the Rapid Texture tool.
3. Set the panel size, or select a contour to serve as a boundary.
4. Set the Displacement parameters and other parameters in the tool.
5. Preview the results (if desired).
6. Apply the texture.
7. Select and position the newly created Rapid Texture contours.
8. Apply a 2D Engrave strategy – making sure to choose the “Follow contour” option.
9. The results will vary depending on the settings of the parameters and the tool that is used to cut the material. 3D Simulation gives a good preview of the look of the finished piece.

Page 354 Texture Tools

Rapid Texture Dialog

Following is a brief explanation of each of the parameters in the Rapid Texture tool. This is followed by some examples that illustrate how the parameters are used to create interesting effects.

Panels Tab


This allows you to save the parameters to a template for later use.


This parameter sets the lower left corner of the panel to the X and Y



This refers to the size of the panels that you wish to create. EnRoute will create a contour to represent the size that has been stated so that it can be cut out and the texture will match up to the next panel.


Refers to the number of panels along the x axis.


Refers to the number of panels along the y axis.


This is the amount that the contours will continue past the perimeter of the panel or selected contour. (Usually at least ½ the width of the tool to be used.) This assures that the tool will continue to cut the texture correctly all the way to the edge of the panel.

Displacement Tab

Wavelength Wavelength is the distance between crests in the texture pattern, both vertically and horizontally. Since the texture pattern introduces “noise” into

the contours, this value is the maximum wavelength used.

Texture Tools Page 355


The distance between the original offset contours. Keep in mind the size of the tool that you are planning to use when you set this parameter.

Horizontal & Vertical Amplitude

Amplitude defines the height of the noise wave, both above and below an axis defined by the offset contours. Amplitude is defined both horizontally (x-y plane) and vertically (z plane).




Displacement provides two options for how the offset contours are modified. The Noise option utilizes a method to distort the contours in a non-uniform way. This option works together with the Randomize option to allow you to create very interesting results. The wave option creates a uniform pattern using the wavelength and amplitude parameters.

Note: When the Wave option is used, the Horizontal Amplitude parameter is used to define an offset of the wave pattern between adjacent contours.


Randomize affects the result when the Noise Displacement option is selected. With Randomize selected, contours are distorted using the noise pattern differently for each contour. This creates a jumbled effect that, when used with the shape of the tool, creates interesting textured

surfaces. When Randomize is turned off, the contours are all distorted using the same noise pattern for all contours.


This option allows you to create a surface panel that is symmetrical in both the x axis and the y axis. That is, its pattern repeats along its edges. This allows you to create multiple pieces that are all alike, but when placed adjacent to each other create a continuous textured surface. In order for this option to work correctly, other parameters must be defined correctly also.

With the Symmetric option, it is usually best not to select a seed contour. Let EnRoute create the straight see contour it needs.

Displacement: Noise should be selected. Randomize should be selected.

Overlap should be defined to ensure that the texture extends off of the defined panel.

Page 356 Texture Tools

Parameters Tab

Fade Left

This parameter allows you to define a distance over which to fade out the Rapid Texture effects on the offset contours. In Rapid Texture, the seed contour is first offset by the specified amount and then the offsets are distorted based on the Rapid Texture parameters. Fading provides anther creative tool for adding new effects with Rapid Texture.

Fade Right

This defines a fade distance to the right of the seed contours, making it possible to have different fade distance on both sides of the seed contour.


Rapid Texture contours are modified using a noise texture pattern. This noise pattern has a resolution that can be defined here. In previous versions of EnRoute, this resolution was fixed at 25 dpi, and this resolution seems to work well for most applications. For very small designs you may want to increase the resolution in order to refine the noise pattern. This will increase the number of segments in each path.



After the offset contours have been distorted using the noise pattern, they are cleaned up in order to reduce the number of points that define each contour. Larger tolerance values will allow you to reduce the number of points in each contour, but this will also reduce the smoothness of the contours. As with other contours in EnRoute, a cleanup tolerance of 0.01 inch to 0.001 inch typically works best.

Texture Tools Page 357

Step by Step Examples

Straight Line Example

Many different textures can be created with the Rapid Texture tool. The following example is a demonstration of a Rapid Texture created with a straight line as the seed contour.

1. Draw the straight line with the line tool.
Select the line.
Click on the Rapid Texture icon to open the tool. 
Enter the parameters:
Size = This refers to the size of the panel you wish to create.
Overlap =0.5
Wavelength = 3
Horiz. Amplitude = 0.4
Vert. Amplitude = 0.2
Offset = 0.2
Select Noise and Randomize

2. Click on the Preview Button. This will show the contours in green and the outline of the panel in yellow. The preview allows you to adjust the parameters until you are satisfied with the results.
Click Apply.
Note: It is not necessary to
preview the Rapid Texture contours before applying them. If you are
confident that you have the correct
parameters, you can just click the
Apply button.

Page 358 Texture Tools

3. The contours will overlap the panel outline by the amount that you entered in the overlap parameter. This allows for the tool to follow the path of the contour through the
edge of the panel, ensuring that the texture will continue to the edge of the panel.

4. The contours are automatically positioned in the plate in the z axis so that the top of the contour is at the top of the plate. It may be desirable to move than down slightly further into the plate in order to ensure that the surface is created properly.

5. Select the contours and add a 2D Engrave toolpath to the contours. In this example a 1- inch Ball End Tool was used.
Make sure that the Follow contour
parameter is checked.

Texture Tools Page 359

6. This is a simulated view of the toolpaths using a 1- inch Ball End tool. A Routing Offset toolpath was applied to the outline contour to cut out the panel.

7. This image shows the same contours but this time a 120- degree Conic tool was used. You can see that the shape and size of the tool can make the texture results very different.

Page 360 Texture Tools

Curved Line Example

1. This example shows the use of a

curved line as the seed contour. Select the contour.

Click on the Rapid Texture icon to open the tool. 
Enter the parameters: Overlap =0.5
Wave Length = 3.0
Horiz. Amplitude = 0.2
Vert. Amplitude = 0.2
Offset = 0.2
Check Noise and Randomize

2. Click on the Preview button. This will show the contours in green and the outline of the panel in yellow. The preview allows you to adjust the parameters until you are satisfied with the contours.
Click Apply.

Texture Tools Page 361

3. The contours are created with the defined overlap.

4. In this image the seed contour is located in a different position and is shorter.
As you can see from the preview and then the contours, if you are trying to texture the entire panel, you would need to lengthen the seed contour so that the offset contours will cover the entire area of the panel.

Page 362 Texture Tools

5. Move the contours to the desired position vertically. Then select the contours and add a 2D Engrave toolpath to the contours. In this example a 1- inch Ball End Tool was used.
Make sure that the Follow contour
parameter is checked.

6. A Routing Offset toolpath is applied to the outline contour to cut out the panel. You can then simulate the toolpaths with the Simulate Ortho tool  to get a good idea of how the texture will look.

7. Once again, we have used the same contours but we have changed the tool to 120- degree conic tool. The simulation tool allows you to see the difference that the tool used will make in the final texture that will be cut.

Texture Tools Page 363

Example with Closed Contours

Closed contours can also be used with the Rapid Texture Tool to create interesting textures and designs.

1. Create the closed contours with the drawing tools.
Select all of the contours.
Click on the Rapid Texture icon to open the tool. 
Enter the parameters: Overlap =0.5
Wave Length = 3.0
Horiz. Amplitude = 0.2
Vert. Amplitude = 0.2
Offset = 0.2
Check: Wave, Randomize.

2. Click on the Preview button. This will show the contours in green and the outline of the panel in yellow. The preview allows you to adjust the parameters until you are satisfied with the contours.
Click Apply.

Page 364 Texture Tools

3. The contours have been created.
Notice that the contours continue past the outline of the panel the distance that was entered in the overlap parameter.

4. Move the “seed” contours to the side and select the contours to be toolpathed.

5. Apply a 2D Engrave toolpath to the contours. Be sure to check the “Follow Contours” box.

Texture Tools Page 365

6. In this example, a 1- inch Ball End tool was used.
To get a good idea of how this pattern will look a simulation of the
1-inch Ball End tool was done. Click on the Simulate Ortho icon to
open the tool. 
A Routing Offset toolpath is used to cut out the panel

Using a Relief with the Rapid Texture Tool

A relief can be used to create even more interesting textures. Simply create a relief and select it along with the seed contour when using the tool. The contours will follow the height of the relief while following the seed contour to create the Rapid Texture.

1. Create the relief to use as part of the texture design. This can be anything from a simple shape to a logo design.
2. Create the seed contour to be used to create the texture.
Select the seed contour and the relief.
Click the Rapid Texture icon to open the tool. 

Page 366 Texture Tools

Enter the parameters: Overlap = 0.2
Wave Length = 2.0
Horiz. Amplitude = 0.2
Vert. Amplitude = 0.2
Offset = 0.2
Check: Noise and Randomize

3. The contours are created and an outline contour is created to follow the path of the panel size.

4. Move the seed contour and the relief to the side and select the contours that are to be toolpathed.
If desired, move the contours down a little in the Z axis.
Apply a 2D Engrave toolpath to the contours. In this example a
1/2'” Ball End was used. Be sure
to check the “Follow Contours

Texture Tools Page 367

5. The Simulate Ortho tool
allows you to create a rendered view of the toolpaths that were applied. A ¼” End Mill tool was used to cut out the panel.

6. This example shows the same toolpaths but the tool has been changed to a 120-degree Conic Bit.

Creating Rapid Texture within a selected contour

EnRoute can also create Rapid Texture contours within a selected closed contour. This feature removes the limitation of creating just rectangular surfaces with Rapid Texture. It can also be used with reliefs to make your 3D surfaces more interesting.
1. Draw the contour and the seed contour.
2. Select the seed contour and click on the Rapid Texture Icon to open the tool. 

Page 368 Texture Tools

3. Click on a closed contour to use as the boundary for your texture. Notice that the contour will be highlighted.
Enter the parameters: Overlap =0.2
Wavelength = 0.5
Horiz. Amplitude = 0.2
Vert. Amplitude =0.2
Offset = 0.1
Check: Wave, Randomize

4. This is a preview of the contours that will be created with the parameters that have been entered.

5. Click Apply to create the contours.
Notice that the contours have only been created within the selected closed contour allowing only for the Overlap parameter of 0.2.

Texture Tools Page 369

6. Select the contours and apply a 2D Engrave toolpath. In this example we have applied a 90-degree Conic tool.
Be sure to check the “Follow contour” parameter.

7. Apply a Routing Offset toolpath to cut out the shape.

8. The Simulate Ortho tool was used to simulate the look of the toolpaths. You can see that the contours extended past the edge of the closed contour shape. This allows the tool to reach all the way
to the edge of the design.

Page 370 Texture Tools

Creating and Cutting Continuous Panels

EnRoute has the ability to create panels that continue the design of the texture over several panels. One example of this type of panel application would be an entire wall that is designed to have a distinctive design. EnRoute makes it easy to create a large Rapid Texture design and continue it seamlessly over several panels.
Following is a very simple example intended to illustrate how to make a continuous surface over several panels.

1. Make the size of the plate the same size as the area that you are applying the textured panels to.
2. Make the size of the panels a little smaller than the size of the material that you are working with.
3. Create the seed contour
In this example, the plate size is 9” x 9”.
The sizes of the panels are 5” x 5”.
4. When you are creating panels you need to determine the size of the panels that you want to create. It is usually just a bit smaller than the size of the material that you will be working with. This allows for the edges of the material to be trimmed so that you can assure a continuous pattern.
Size = 5” x 5” –This is the size of each panel.
Wave Length = 5.0
Horizontal Amplitude =0 .6
Vertical Amplitude = 0.3
Offset = 0.4
Rows = 2 Columns = 2 (This represents the number of panels required for the finished area.)

Texture Tools Page 371

5. Once you have entered the parameters, click on the Preview button. The preview will be drawn on the screen. You can get a good idea of parameters that you have set. The green represents the contours that will be created. The pink and yellow represent the contour that outlines the panels that you have created.

6. Click Apply to place the contours.
You will notice the contours are continuous over the length of the panels.
The next step is to apply toolpaths and then cut the panels. To do this, there are some things that you need to consider.
The size of the plate will need to reflect the size of the material that you will be cutting the panels from.
Each of the panels will need to be individually cut because of the uniqueness of each panel.
We suggest that you create layers for each of the panels. You will need to take care in labeling the panels when placing them on the layers because when you install the panels, you will need to know where each panel is located relative to the others.

Page 372 Texture Tools

7. Change the size of the plate to reflect the size of the material that you are working with.
Click on the Plate icon to open the
Define Plate Dialog. Enter the parameters
to reflect the size of the material that you are using to cut the panels.
In this example the plate size was changed to 5.5 x 5.5.
Note: Your projects will most likely use much larger panels. This small size was used for illustration.

8. From this graphic, you can see that the texture contours and the outline contour for each panel are separate from the adjoining panel.
Systematically go through and create new layers for each panel and then move a copy of the panel contours to the specific layer associated with the panel that you have copied.

9. To create a new layer, click on the Define
Layers Icon or press F7.
Click on the New button. This will create a new layer. Highlight the layer name and type in a name for the layer that you can associate with the panel that you will be cutting. It is important to be careful when naming the layers and then copying the correct panel to that layer. You will need to know the locations of the panels for installation.

Texture Tools Page 373

10. Once you have the new layer created, copy the panel outline and contours and paste to active layer.
From the image shown, you can see that
the contours will be copied to the layer but in the same position that it was on the original layer.
To move the contours to the Center of Plate, press Ctrl + 5.

11. Notice that the contours are now in the center of the plate. This will allow room for the texture contours to continue off the end of each panel. The reason is to make sure that the textures will line up with the next panel accurately.

Page 374 Texture Tools

12. Continue to create and copy each panel to the correct layer.
Your layers Dialog may look something like this when you have finished.
Each panel should be copied to the correct layer and moved to the center of the plate to be toolpathed.

13. The next step is to toolpath the contours for each layer. Apply a 2D Engrave toolpath to the contours. Be sure to check the Follow Contours box.
Use the same tool for all of the panels to assure the consistent look of the finished product.
Be sure to mark each panel as you cut it so that it can be installed in the proper position.

Texture Examples

Below are a few textures that EnRoute is capable of creating. These textures are just a few examples of the unlimited designs that you can create.

Symmetric Texture

A symmetric texture creates a rectangular texture that is symmetric left to right and top to bottom. This allows you to cut several pieces, each of them identical, and they will match up along their edges.

The Parameters for this texture are as follows: Size X: 6.00
Size Y: 6.00
Overlap: 0.1
Wave length: 3.00
Horizontal Amplitude 0.35
Vertical Amplitude 0 .20
Offset 0.20
Noise = checked
Randomize = checked

Texture Tools Page 375

Symmetric = checked

The seed contour for a symmetrical texture is always a straight line contour. The tool used to cut this texture is a 1” ball end tool. The toolpaths that have been created follow the curve of the seed contour.

This is an image of the contours that were created with the parameters listed above.
In order for the symmetric texture to work correctly, the settings for the wavelength parameter must divide evenly into the size of the X size.
The settings for the Offset parameter must divide evenly into the size of the Y size.
The image below illustrates how the contours line up at the edges of the piece. The contours
were copied and moved to the side of the existing contours. You can see that they line up exactly.

Page 376 Texture Tools

This is a close up view of the point where the contours meet.

Basic Noise Texture

The parameters used to create this texture are: Overlap = 1.0
Wavelength = 2.0
Horiz. Amplitude = 0.3750
Vert. Amplitude = 0.25
Offset = 0.15
Noise = checked
Randomize = checked
A straight line contour was used as the seed contour. A ½ ball end tool was used to cut the texture.

Chip Texture

The parameters for the Chip Texture are: Overlap = 1.0
Wavelength = 1.0
Horiz. Amplitude = 7.0
Vert. Amplitude = 0.25
Offset = 0.25
Noise = checked
Randomize = checked
A straight line was used for the seed contour and a 1-inch Ball End tool was used to cut the texture.

Texture Tools Page 377

Chip Texture 2

The parameters for this texture are: Overlap = 1.0
Wavelength = 0.7
Horiz. Amplitude = 1.0
Vert. Amplitude =0 .25
Offset = 0.20
Noise = checked
Randomize = checked
This texture was cut using a 1-inch Ball End tool.

Wavy Noise Texture

The parameters for this texture are: Overlap = 0.1
Wavelength = 3.0
Horiz. Amplitude = 2.0
Vert. Amplitude = .01
Offset = 0.25
Noise = checked
The seed contour used was a straight line contour. The toolpaths were cut with a 90- degree conic tool.

Page 378 Texture Tools

Wave Texture 1

The parameter for this texture are: Overlap 1.0
Wavelength = 3.0
Horiz. Amplitude = 1.5
Vert. Amplitude = 0.2
Offset = 0.7
Wave = checked
A straight line contour was used as the seed contour and a 1-inch Ball End tool was used to cut the toolpaths.

Wave Texture 2

The parameters for this texture are: Overlap = 0.1
Wavelength = 2.5
Horiz. Amplitude = 1.0
Vert. Amplitude = 0.2
Offset = 0.5
Wave = checked
A straight line contour was used as a seed contour and a 90-degree conic tool was used to cut the toolpaths.

Texture Tools Page 379

Rapid Picture Tool

A photograph can be used along with the Rapid Texture tool. In this tutorial we will demonstrate the use of photo images used to create a lasting remembrance using the rapid picture tool.

Selecting a Photo

In this example, a black a white photo was used. We have found that a color picture usually works best because the tone of the picture is not as uniform as a black and white photo. So some changes were made to the photo to enhance the contrast of the original photo. Below the first picture is the original, the second picture is the one that was used in this example. We tried to create more of a contrast between the light and dark areas of the photograph.

Page 380 Texture Tools

1. Start with opening a new EnRoute file.

To do this click on the New icon.  This will open the Define Plate Dialog.
Enter the parameters. Width = 15.00
Height = 15.00
Width = .50
Click OK.
This will create the workspace for your design.
2. The plate will be shown in red. 

3. Import the photo into the workspace using the Import tool.
Click the Import icon
Find the file that you wish to import. Click on OPEN.
This will import the picture to your workspace. The imported picture will create another layer called “Imported”. Both of the layers will be turned on and you will be working in layer 1.

Texture Tools Page 381

4. The next thing we did was size the photo.
Select the Photo.
Press the F2 button. This will open the
Precision Input Dialog. Enter parameters: Width = 13.00
Height = 13.00
Click OK.

5. Notice the image is located at the bottom left of the plate. Move the image to the center of the plate.
Click on the image.

Note: Hold down the Ctrl and Alt Key and press the number 5 in the 10 key keyboard to move to the center of the plate.

The image is now in the center of the plate.

6. Using the rectangle tool and the snap tool you can quickly place a contour at the edge of the plate.
Click on the Snap to Grid icon. 

Note: The settings for the grid have been set at 1 inch intervals.

This will turn on the snap feature.
7. Click on the Rectangle icon. 
This will open the rectangle tool. Make sure that the construct rectangle by corners is selected. 
Move the cursor to the top left corner of the plate, click to place the first corner. Drag the cursor to the bottom right corner of the plate and left click to place

Page 382 Texture Tools

the opposite corner of the rectangle. This will place the contour needed to
apply the Routing Offset toolpaths to cut
out the design. (The toolpath will be applied later.)
The next step is to create the contours for the photo image.

Creating the Seed Contour

The drawing tools are used to create the “seed contours” for the rapid texture design. The seed contour is the starting point for the Rapid Texture process. If you don’t define a seed contour, EnRoute will define a straight one for use within the tool. When the Rapid Texture contours are created, they are first created as offsets from the seed contour based on the Offset parameter in the Rapid Texture dialog. The offsets are then distorted using the other Rapid Texture parameters, creating the finished Rapid Texture contours. Since the seed contour is the starting point, it is an important part of the design process. Seed contours can be virtually any shape desired; they can be open or closed contours; and, you may select more than one seed contour at a time. Whatever contours that are currently selected when the Rapid Texture process is started are used as the seed contours. With some experimentation you will find that even using all of the same parameters, you can change the end result of the Rapid Texture results quite dramatically simply by changing the shape and number of seed contours selected.

8. Draw a straight horizontal line across the plate. This is the contour that will be used as the “seed contour”.
9. Click on the line and open the Rapid 

Texture tool.

Texture Tools Page 383

10. Click on the photo image. This will open a dialog box that will allow you to select the tool that will be used to cut the toolpaths. In this example we have chosen to use a .02 Engrave tool.
Click Accept.

11. The whitespace gap parameter refers to the minimal space that will be between the contours in the dark portions of the photo. The surface of the material will reflect this parameter when it is cut.
Enter .020
Click OK.

12. This information dialog box recaps the information that you have entered for this project.
Review the information and Click OK.

13. Set the parameters for the Rapid
Position: X = 1.00
Y = 1.00
The position parameters refer to the start point of the panel that will be designated as the area where the rapid texture contours are created. We entered the start point at 1 inch because we want to have a 1-inch border around the rapid texture design.

Page 384 Texture Tools

14. Set the Size parameter: Size X = 13.00
Y = 13.00
Overlap = 0.00
The size parameter refers to the size of the panel that we wish to create for the rapid texture contours.
The overlap parameter refers to the distance that the contours will continue outside of the panel.

15. Wavelength = 3.50
Horiz. Amp = 1.50
Vert. Amp = .01

16. Offset = .15.
This parameter refers to the distance between the contours.
Displacement Noise = Checked Click Apply.

17. The contours will be created.
This is a close up view of the contours that have been created.

Texture Tools Page 385

18. The contours are created within the area that you have set for the panel

19. The next step is to apply the toolpaths to the contours. Select the contours.
At this point the contours are grouped so you can just click on one of the contours and they will all be selected.

20. Click on the Engrave icon. 
This will open the Engrave dialog. Enter the parameters:
Select the .02 Engrave tool
Depth = .10
Follow Contours = checked
Set the feed rate to 60 inch per minute
Click OK.

Note: The slow speed helps to eliminate chipping of the material we were using. Feel free to adjust this to fit your machine and material.

Page 386 Texture Tools

21. This image shows the toolpaths that have been applied.
Next it is a good idea to group the toolpaths while they are selected.
Click on the Group icon. 
22. The next step is to apply the Routing

Offset toolpaths to the panel contour.
Click on the Routing Offset icon.
Enter parameters:
¼” End Mill
Depth = .50
External = checked
Click OK.

23. An Engrave toolpath is also added to this same contour in order to put a beveled edge on the design.
Click on the Engrave icon.  Enter parameters:
90 Conic Tool
Depth .20
3D Engrave toolpath = checked
Internal = checked

Texture Tools Page 387

Click OK.

24. Use the Simulate Ortho tool to create a rendered view of the toolpaths that you have created.
Click on the Simulate Ortho icon. 
25. You are now ready to cut your project.

Page 388 Texture Tools

20.Relief Edit Tools

The Relief Editing tools provide a quick and simple method for editing any relief surface using tools that are similar to bitmap painting tools. This provides another powerful creative tool for relief creation.
There are five tools to use to edit your existing relief or to use to create a new relief using the mouse to draw a free hand design. The same basic concept of Add, Subtract, Merge Highest, Merge Lowest and Replace are used in combination with the shape of the tool specified.

Edit Relief Toolbar

Menu: Surface / Relief Edit

Toolbar: 3D Surfaces / Edit Selected Relief

These tools are found in the Surface Menu under Relief Edit or in 3D Surfaces Toolbar by selecting the Edit Selected Relief tool. 


Smooth Relief Edit Tool – This tool is rounded at its top and base so it works well to gently modify a relief surface.

Bevel Relief Edit Tool – The bevel shape on this tool is great for adding details to your surface.

Dome Relief Edit Tool – This tool has an arc shape.

Flat Relief Edit Tool – This is good for interactively adding a specific amount to your surface.

Blended Relief Edit Tool – This tool is used to blend the surface. It will even out the surface within the selected radius.


The radius specifies the size of the tool.

Relief Edit Tools Page 389


This is the angle from the edge of the tool to the center. This is used to define the height of the edit tool.


This specifies the height of the flat tool.

Use Spline

If this option is checked, when you click and drag the mouse to edit the relief, EnRoute saves the points and then uses them to define a smooth curve for the edit. If it is unchecked, then EnRoute uses the points it gets from the mouse directly without trying to smooth them.



If this parameter is checked, each time that you drag the tool over an area of the relief, the surface will be affected by the specific parameters of that tool and add to any prior movements of the mouse with that specific tool.


The fade parameter reduces the radius of the tool from the set size to zero within the stroke of the mouse movement. This allows you to blend with the existing relief.


The shrink parameter affects the height of the tool parameters, reducing it from the highest to the lowest within the mouse movement. This also allows the tool to blend with the existing relief.


Click Apply to accept changes that have been made with an edit tool. These edits can be reversed outside of the edit tool by using undo.


Click the clear button if you choose not to accept the changes made while using the edit tools. If you change tools, the change is accepted for the previous tool. You can use the Undo tool if you do not like the changes to the relief that have been already been accepted.


Click close to exit the tool.

Fade and Shrink

The fade and shrink parameters are used in conjunction with the Spline parameter. Using these parameters will help to blend into the existing relief. One thing to remember is that the larger the radius of the tool and the higher the resolution of the relief, the longer it will take to process.

This shows the bevel tool with the Fade parameter set all the way to the right. The mouse movement was from left to right. The tool edited the relief from the largest to the smallest point.

Page 390 Relief Edit Tools

Build Parameter

This shows the bevel tool with the Shrink parameter set all the way to the right. The mouse movement again was left to right. The relief does not get smaller in diameter, but the height of the relief moves from highest point to lowest point.
The build parameter allows you to use your tools to “build up” a specific area of your relief. In the examples below you can see how the relief is affected with and without the build parameter.

Top View with Build parameter checked. Perspective View with Build parameter checked.

Top view with Build parameter unchecked. Perspective view with Build parameter unchecked.

Relief Edit Tools Page 391

Examples using relief edit tools

This example shows the use of the Relief Editing Tools. The top image is a quick assembly of a violin. Using the Relief Edit tools, you can add details and use the smoothing tool to blend and soften the design.

This image shows small adjustments to the relief.

Page 392 Relief Edit Tools

21. 3D Toolpaths


After creating a relief, the next step is to create the toolpaths you will use to mill the finished piece. Although the results can be quite different, the process of creating 3D toolpaths is largely the same as creating other types of toolpaths in EnRoute. It includes selecting the proper strategy and then defining the tools and other parameters that will be used to create the toolpaths. The difference is that with 3D toolpaths there are a few additional parameters that are required to define how the relief is used to create the toolpaths.
This chapter describes how to use relief surfaces to create 3D toolpaths. It assumes the reader is already familiar with EnRoute 2D toolpath strategies.

3D Toolpath Strategies

3D toolpaths can be created using most of the same strategies that are used for other types of toolpaths. This includes routing offset, hatch fill, island fill, and engrave. The hatch fill and island fill strategies will be the ones you use most commonly since they are the ones that are used to mill the relief surfaces you create. Routing offsets are useful with reliefs to clean up tooling marks on vertical edges in the relief, and the engraving strategy allows you to add 3D engravings on relief surfaces.

3D Toolpaths Page 393

3D Toolpath Strategy Parameter

The parameters that are required for defining 3D toolpaths are activated as part of the standard strategies if you have one or more reliefs selected when you activate that strategy.

The first thing you notice when you activate a strategy with a relief selected is the new checkbox at the bottom of the parameters dialog, named Apply to reliefBy checking this checkbox, you have access to four additional parameters that define how the toolpaths will be applied to the relief.

Apply to Surface

Apply to surface means that the toolpath will follow the surface of the relief and the depth of cut will be adjusted to follow the relief. If the toolpath covers an area with no relief, the depth is defined by the settings in the cut definition. The cut depth defines the maximum depth of the new toolpaths.

Carve into surface

Carve into surface allows the toolpath to follow the relief while using the cut depth information to define how deep to cut into the relief. One of the common uses of this parameter would be to create a

3D Engrave toolpath that follows the surface of the relief while creating the 3D effect into the relief surface.
When you select this option two more check boxes appear.

Project is the most common selection; it calculates the toolpaths as if they were applied/projected onto the relief.

Float calculates the toolpath and makes sure the tool will not remove part of the relief. This can cause distortion of the toolpaths and should only be used in special circumstances, if it is particularly important for the new toolpaths not to gouge into the relief.

Apply Overcut

Overcut amount (Fills Only) allows EnRoute to compensate for the characteristics of the ball end mills used to create 3D objects. Without this parameter, the outside edges of your object would have a scalloped effect. Overcut allows the toolpath to be created OUTSIDE the boundaries of the relief to eliminate this problem.

 As a rule of thumb overcut should be set to a little less than ½ the tool diameter on the finish pass.

Page 394 3D Toolpaths

Cut Definition Parameters

In the Cut Definition dialog there are a few more parameters that are new in 3D.

In the Depths section Offset from surface allows you to set how close you want the toolpaths to follow the surface of the relief. Usually this is defined for a roughing pass to ensure that the roughing pass does not damage the finished surface. The offset distance is determined by many factors, including type of material, type of tool (roughing and finish), and how fast you want the roughing pass to run.

The following shows toolpaths with a 0.20 offset.

3D Toolpaths Page 395

Step Rough

This option is available with Hatch and Island fills. It provides an optional method for creating toolpaths to rough out the relief surface prior to creating the finish toolpaths.
The advantage of this method is that it creates 2D toolpaths at multiple pass depths that remove as much material as possible at each pass depth. Because the toolpaths are 2D, they can typically be defined using higher feed rates than 3D toolpaths. Also, each pass only cuts the portions of the relief it can reach, so it is typically more efficient than using multiple passes of standard 3D fills as roughing passes.
The possible disadvantage of this method is that steps are left for the finish pass. The height of the steps is equal to the difference between depths of each pass of the step rough. The ball end mill that is used for the finish pass must be capable of cutting the steps that remain after the step rough.

The first image shows toolpaths with the step rough option. The second image shows a rendered view of these toolpaths.

Page 396 3D Toolpaths

Key 3D Toolpath Concepts

Before you start creating 3D toolpaths there are a few things to consider that mostly do not apply in
2D. You likely already understand that a three- axis router creates 3D objects with a ball end mill that
“steps over” incrementally, making numerous passes at different depths to waste the material around the finished surface. The constraints here are the size of the tool, the amount of overlap, and how much detail is required. The relationship is the smaller the tool, the larger the overlap, the finer the detail, the LONGER the time to cut. EnRoute gives you the control you need to balance these factors so that you can create a high quality finished surface in a reasonable amount of time.
In general, the depths of cut are greater across greater areas of your material. This means you need to be careful to use the visualization tools in EnRoute to be sure your job will cut correctly. The rough tool and the roughing strategies will go a long way toward getting the job done. The reason for roughing is to clear material out of the way for the finish pass to run. You generally want to run the finish cut in a single pass as this pass takes the longest time to run; also, you have a more limited selection of tools for the finish cut. Another thing to consider is the length of the tool in relation to the surrounding material. It is easy to get yourself in trouble trying to get a small tool into a deep area. EnRoute gives you the tools to avoid these situations but you need to be aware that they exist.

3D Toolpaths Page 397


When it comes time to mill out a 3D surface, the selection of the proper overlap percentage becomes quite important. The proper percentage can vary widely depending on the size of the relief, the size of the tool, the type of material being used, and the quality of the finished surface that is desired.
Milling a relief surface requires a ball end mill tool in order to allow you to cut smooth surfaces. The spherical surface of the tool will create small grooves in the finished surface. The size of the grooves will vary depending on the amount of overlap. As you increase overlap percentage the tool marks are reduced, but the time required to mill the surface increases. The goal is to choose an overlap value that balances cut quality with cut time.
The best way to determine proper overlap for a job is to create and cut a test relief using the same type of material as the job. Then you can estimate the duration of the entire job, and see the surface quality, and the amount of finish work that will be necessary to complete the job.
Typical overlap values range from 80% for larger reliefs that don’t require a smooth finish, to 95% for
small reliefs cut from dense material that requires a very smooth finish.

Page 398 3D Toolpaths

3D Toolpath Example

The following simple example illustrates the process of applying 3D toolpaths using the Island Fill

Strategy and Hatch Fill Strategy.

1. Start with a plate size of 4 x 4

x 1.  Draw an oval and a star. Align the objects to center. 

2. Select the Create a Relief


3. Click the Add icon to select that option.

4. Select the Rounded option.

5. Select the Limit to height

Application method.

Define Height = .30

Base =0.00

Resolution = 100

6. Enter the angle parameter as


Click Apply.

7. This is a rendered top view of the object.

3D Toolpaths Page 399

8. Select the relief and hold the Shift key and select the star. Select the Add Icon.

By selecting both the relief and the star, this tells EnRoute to apply the star to the relief rather than creating a new separate relief for the star.

9. Select the Beveled option.

10. Select the Limit to Height

Application Method.

Define: Height = .30

Base =0.00

11. Enter the angle parameter as


12. The rendered view should look similar to this.

13. Select the relief. Click and hold the Align relief icon. Select the Align all reliefs to top of plate option.

14. This will move the relief into the plate vertically. The front view shows the vertical placement of the relief in the plate.

Page 400 3D Toolpaths

15. You may also place the relief precisely by pressing F2 to activate the Precision Input Center.

Click on the Move tab and enter the desired X-position of the relief.

This option works best when the Front view is active, because then the button box selection applies to the X and Z location of the relief.

16. Select Island Fill Add a

¼ inch ball nose tool.

When a relief is selected, the option Apply to relief is activated in the parameters section. Make sure this is checked. Choose Apply to surface and Apply overcut. Enter overcut amount of 0.08.

Usually the overcut amount should be set at a little less than one-half of the diameter of the tool.

17. Click in the edit box for the ¼ inch tool to activate the Cut Definitions dialog.

18. Enter a final depth of 0.60.

19. Enter fill overlap of 85%. For a finished surface, the overlap percentage will typically vary between 80% and 95%, depending on the material, and

3D Toolpaths Page 401


the quality of the finished surface that is required.


20. Enter number of passes as 1.

In this example we are not defining a rough cut tool, and the assumption is that the ¼ inch ball end mill tool will be capable of cutting the full depth of the relief in one pass.


21. Click Ok to return to the Island Fill Dialog. Click OK to calculate the tool paths.

This is the top view of the

Island Fill tool paths.

22. This is the front view.

To cut the object from the material, a Routing Offset toolpath would be defined.


23. This example shows the same relief with Hatch Fill toolpaths applied. The same parameters have been applied when defining the toolpaths.

The preferred strategy would be determined by the type of material used. The cutting time in this instance would likely be shorter with the Island Fill strategy.


Page 402 3D Toolpaths

3D Toolpaths with a Step Rough

This next example demonstrates the application of toolpaths to a larger and more intricate design. This type of relief requires a little more thought when creating toolpaths. Because it is deep, it likely
isn’t possible to cut it out using one tool. Therefore, it is necessary to create one or two roughing passes to remove the bulk of the waste material prior to running the finish toolpath.
The first cut we add is a rough pass. The primary purpose of this cut is to remove material efficiently. The step rough option allows for the most efficient removal of material.
The following relief will be cut using the Island Fill strategy. The first pass utilizes the step rough feature. This allows for most of the material to be cleared away prior to the finishing passes. The parameters are defined as follows.

1. This is the top view of the relief that will be toolpathed in this example.

The size of the relief is approximately 12 x 15 x 2 inches.

2. This is the Front view of the relief in this example.

3. A 3/8-inch end mill tool is used for the step rough toolpaths.

3D Toolpaths Page 403

The following parameters were entered to create the Island Fill toolpaths.

4. Select the following: Apply to Relief

Apply to Surface

Apply Overcut

Overcut amount = 0.50

5. Define the Depths as: Surface = 0.00

Final Depth = 2.0

Offset from surface = 0.20

Step Rough = checked

6. Overlap of 75%.

Corner tags = unchecked

7. Passes are defined as: Number = 8

Maximum per Pass = 3.0

Actual per Pass = 0.25

Final Pass = unchecked

Final Pass Depth = 0.00

8. The following feed rates are defined. This part is to be cut from Western Red Cedar, which is a soft wood that is prone to chipping.

Feed Rate = 220.00

Final Pass Feed = 0.00

Plunge Rate = 100.0

Dwell = 0.00

Spindle = 18000

9. Select the Climb direction.

Page 404 3D Toolpaths

10. The toolpaths for the 3/8-inch tool are shown here.

11. This image shows a rendered view of the step rough toolpath using the

3/8-inch tool.

3D Toolpaths Page 405

Roughing Pass

The next step in defining the toolpaths for this relief is another roughing pass. The second cut to add is another rough cut. The purpose here is to create a surface that is closer to the finished surface than the step rough. One disadvantage of a step rough is that it creates a surface with ledges that may be too tall for the finish tool we will use. A standard roughing pass will create a relatively smooth surface.

12. Select the Island Fill Strategy and a ¼ inch end mill tool for this cut.


13. Select the following: Apply to Relief

Apply to Surface

Apply Overcut

Overcut amount = 0.50

14. Surface = 0.00

Final depth = 2.00

Offset from surface = .10

Step Rough = unchecked

15. Overlap = 75%

Corner tags = checked

An overlap of 75% gives a relatively smooth surface without requiring too much time to cut.

16. Passes, Number = 1

Maximum per Pass = 2.1

Actual per Pass = 2.0

Final pass = unchecked

Final Pass Depth = 0.0

17. Feed Rate = 280.0

Final Pass Feed = 0.00

Plunge Rate = 100.0

Dwell = 0.00

Spindle = 18000

Page 406 3D Toolpaths


18. Select the Climb direction.


19. In the perspective view; you can see that we have created one pass that follows the surface. Notice that the toolpaths are not directly ON the surface. This is because we used an end mill and

the program calculates to the edge of the tool but the toolpaths are displayed as centerlines. Normally the roughing pass would be set up with an offset, which creates a toolpath that keeps the edge of

the tool away from the relief by the offset amount. In this example we

used an offset amount of 0.10 inch.


20. This is the front view of the roughing pass toolpaths.


21. This is a rendered view of the step rough pass and the roughing pass toolpaths.

3D Toolpaths Page 407

Finish Pass

The final step in cutting this relief is to add the finish pass. For this pass a 1/8-inch ball end mill tool has been defined. You can create one strategy that includes both the roughing and finish passes, but you may prefer to create them separately since this can allow easier visualization and control later.

22. Select the following: Apply to relief

Apply to surface

Apply overcut

Overcut = 0.10


23. Surface = 0.00

Final depth = 2.0

Offset from surface = 0.00

Step Rough = unchecked

Notice with the finish pass that the offset is set to 0.00.

24. Overlap = 88%

Corner tags = unchecked

25. Passes: Number = 1

Maximum per Pass = 2.10

Actual per Pass = 2.0

Final pass = unchecked

Final Pass Depth 0.00

26. Feed Rate = 360.00

Final Pass Feed = 0.00

Plunge Rate = 100.0

Dwell = 0.00

Spindle = 18000

27. Select the climb direction.

Page 408 3D Toolpaths

28. This is a rendered view including all toolpaths.

29. This is a close-up view of the 3D toolpaths. Rotate it in perspective and you will see the dense

pattern of your finish pass

toolpaths. The appropriate overlap amount varies depending on the material you are cutting, the amount of cleanup work you want to do, and the length of time you have to run the job. Values

of 75% (coarse) to 95% (fine) are typical. The higher the overlap

the more time the job will require to run. We suggest that you experiment by running the same relief at different overlaps to get

a feel for the time and texture.

3D Toolpaths Page 409

Engrave Toolpaths on a Relief

This next example shows the application of 3D toolpaths applied directly to a relief.

1. In this example the plate size is 4 x 6 x

1. The object is a 4 x 6-inch rectangle.

2. Select the rectangle. Create a relief  using the following parameters:

Add to relief Rounded relief Normal Resolution = 100

Angle = 50 degrees

3. The results should be similar to this perspective view image.

4. Move the relief into the plate.

Select the relief. Click and hold the Align relief icon. Select the Align all reliefs to top of plate option.

5.  Add a text object to the design.

Center the text object with the relief.

Page 410 3D Toolpaths

6. Select both the relief and the text


Select the Engrave toolpath icon.

Add a Conic Tool with a Depth of .10.

7. Select the following:

3D Engrave toolpath


Apply to relief

Carve into surface.

The parameter here is the choice to carve into the surface rather than to apply to the surface.

8. After entering the appropriate strategy and cut parameters, click OK in the strategy dialog to create the toolpaths.


9. Look at the job in the Perspective view and see how the contours stay at the top of the plate while the toolpaths follow the underlying relief. This tool allows us to create a 2 1/2D toolpath along a 3D object. Remember, a key to this technique is to select the relief as

well as the object when you first activate the toolpath dialog.

10.  This is a rendered view of the object after the relief surface has been toolpathed using a hatch fill and the engrave toolpaths have been applied.

Notice how the engraved word follows the curve of the relief.

3D Toolpaths Page 411

Routing Offset

1. Use the same relief as in the previous example to create a routing offset toolpath. In this example, you will see that creating

a routing offset to cut out

a relief is no different than creating any other type of

routing offset.

2. Select the relief. Select the Routing Offset icon. Add a ¼ inch End Mill tool, with a depth of


3. Select the External


4. In the cut parameters dialog for the ¼” End Mill tool, change the number of passes to 3.

Click OK to get back to the strategy dialog.

In the strategy dialog, click OK to create the routing offset toolpaths.

5. The perspective view is a good way to view the toolpaths.

Page 412 3D Toolpaths

6. This is a rendered view of the final object. It includes the fill and engrave toolpaths from the previous example.

3D Simulation of Toolpaths

This tool displays a rendered 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. From the Output toolbar, select Create Rendered Simulation of Toolpaths. 

3D Toolpaths Page 413

2. This will activate the Simulate Ortho toolbar, and it will also bring up the Sim Options dialog.
The dialog lets you define all of the parameters associated with the simulation. You can get a detailed explanation of this dialog in Chapter 9.

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.

Page 414 3D Toolpaths

to the one in the Output dialog.
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.
4. Click Done to end the simulation.
 Be sure to activate the Rendered View icon .

Image with rendered view activated.

3D Toolpaths Page 415

Page 416 3D Toolpaths

22.Automatic Toolpaths


EnRoute’s Automatic Toolpath (ATP) capabilities allow you to process parts contained in external DXF geometry files. This type of geometry is commonly generated by design applications that serve industries such as the cabinetmaking and furniture making industries.
EnRoute’s Automatic Toolpath capabilities provide an efficient way to process large numbers of parts
as part of a Nested-Based Manufacturing (NBM) process.
This chapter provides a description of EnRoute’s ATP capabilities, including a description of how to set up the required configuration settings, how to set ordering and output preferences, and then how to process files.
The following graphic shows a sheet of nested parts that have been processed using EnRoute Wood.

Automatic Toolpaths Page 417

Design Application Support

Several design applications are supported by EnRoute Wood, and new application support is added based on requests from users, manufacturers and customers. The list of supported design applications is continuously being updated to reflect new applications.

Editor’s Note: The graphics in this Automatic Toolpath discussion must often show a particular design application as the active application. In the interest of simplicity, KCD was selected as the active application to show in most of these graphics. This is not intended to offer a specific recommendation or to exclude any of the supported applications. References to the active application in the text are either represented as <active application> or <KCD> and should be interpreted to mean that any of the design applications can be inserted into these references.

Overview of the ATP Process

When DXF files are created in the design applications supported by EnRoute, different types of machining operations are separated onto different layers in the DXF files. The geometry on all the layers in a file represents a single part, and all of the machining such as drilling, milling, and cutting, that is to be performed on that part. In order to process the part, the ATP needs to be instructed about what operations (Strategies) should be applied to each layer of geometry in each DXF file.
When EnRoute processes a part, it uses this mapping of toolpath Strategies to apply toolpaths to each piece of geometry in the part. After all the parts have been imported and had toolpaths applied, they are nested together onto sheets and then machining output files are created based on the ordering and output preferences defined.
At first, this process may appear to be rather complicated, but the nice part is that after you have defined the desired parameters for Layer/Strategy mapping, ordering and output they can be saved in an ATP configuration file. Then when it is time to process another job the ATP file can be opened to recall all of the desired settings. As few as three mouse clicks can be required to process a job that may contain dozens of parts.
The following diagram shows the general flow of tasks utilized to process an Automatic Toolpath job.

Page 418 Automatic Toolpaths

Automatic Toolpath Process

Select the Design Application

This only needs to be set one time.

Select Files to Process
Map Layers and Strategies

Select Ordering and Nesting Params

These steps can al l be saved in the ATP file so t he y ca n be com pl et e d simply by loading a saved A T P p a r a m e t e r f i l e .

Select Output Options
Process Files

Activating the ATP Dialog

The ATP dialog is activated by selecting the File menu and clicking on Automatic Toolpaths. It can also be activated by clicking on the Automatic Toolpath button located in the Output toolbar.

Automatic Toolpaths Page 419

The ATP Dialog

All of the ATP functions are contained in one dialog. The tabs in the dialog represent the major steps that were introduced in the ATP overview previously. Initially many of the parameters in the ATP dialog are blank. When a saved ATP parameter file is loaded, this dialog is filled out based on the parameters in the ATP file. The next several sections provide a step-by-step discussion of the process of defining the required layer mapping and other parameters required to successfully
process parts using the ATP.

Dialog Tabs

Processing Buttons

Processing Buttons

There are seven buttons that are present all the time that the ATP dialog is active. This is because these functions can be activated at any time. These buttons are highlighted above.

Load – This activates a load dialog for loading a saved ATP file. ATP files may be located anywhere that is most convenient the same as standard EnRoute drawing files.

Save – This allows you to save the current parameters into an ATP file. If an ATP file has been previously saved or loaded during this ATP session, the file will be saved without prompting you to identify where, and by what name, to save the file. If the file has not been previously saved, you will be prompted to name the file to save.

Save As – This is the same as the Save button, except that it always activates the save dialog to prompt you for a name under which to save the file.

Close – This closes the current ATP session, and returns you to the EnRoute environment. If changes have been made to current ATP parameters, you will be asked whether to save these changes as the active ATP parameters. If you click on Yes, the current parameters will be saved in EnRoute’s memory so that if you get back into the ATP these parameters will be restored.

Page 420 Automatic Toolpaths

There are three Process Buttons that tell EnRoute to use the current ATP parameters to process part information. The difference between these buttons is that they each tell EnRoute to process different part information. Very likely you will utilize just one of these buttons for a majority of your work, depending on how your part information is processed.

Process Active – This processes the active EnRoute drawing. This is the drawing that was active when you started the current ATP session. For most users, this option will not be utilized very often, but it can be convenient if you would like to quickly process some parts that you have created in EnRoute, or imported from another application.

Process Files – This button processes a list of DXF files that you have identified in the list shown in the ‘Select Files’ tab. This option allows you to process geometry files that have been created by a separate design application that may not be directly supported by the ATP. For example, many users utilize AutoCAD to generate their designs, and then would like to process these designs in EnRoute. This option makes it easy to accomplish this task.

Process <Active Design Application> - This button processes the files that have been specified for the active design application. The button text changes depending on which design application is active. For example, if KCDw is the active design application, the button will read ‘Process KCDw’.

Selecting the Active Design Application

If you are using one of the supported design applications, this should be set first before starting the process of defining the layer mapping and processing files. After this has been set, EnRoute will remember this setting so it won’t be necessary to define it again unless you change design applications.
To set this parameter, click on the Setup tab and select the desired application from the list in the dropdown as shown below.

Automatic Toolpaths Page 421

Note - Notice that it is possible to select No active application as an option too. If this option is selected, then individual DXF files may be processed in pretty much the same way as if they came from a supported design application. One key difference is that information about the size, material and orientation of the parts won’t be available to interpret as part of the processing.

Selecting Files to Process

After the design application is specified, the next step is to select which parts are to be processed. The output created by each of the supported design applications includes a List File that is a list of all of the separate DXF files in a job.
For example, if you have used KCDw to design a set of kitchen cabinets and then output this geometry to be processed in the ATP, each part is represented by a separate DXF file. The List File for that job is a table that lists all of the DXF files in that job along with additional information such as the size, material, quantity and rotation for each part.
EnRoute allows you to import List Files which load part information for each of the parts in the job. The presence of each of the DXF files is automatically verified, and the information about the parts is shown in the table.
To select a list file, first click on the Design Application tab in the ATP dialog. This tab will have the name of the active design application (AllMaster Software, Pathfinder, etc…). Then click on the Add List File button, which will activate an Open File dialog. This dialog will look specifically for files that match the extension of the list file for the active application.

Select List File Tab

Page 422 Automatic Toolpaths

List Files for the active application in the current folder

After the List File loads, the parts are shown in the table. The dialog shows the total number of parts to be processed. If you process a job after a List File has been imported, the parts will be created just as they were specified. As an option, some of the parameters about the parts may be modified if desired. It is not possible to change such things as the size of the part, but you can change the quantity of each part, turn off the processing of selected parts, or custom rotate individual parts.
The following screen capture shows the table after it has been populated with the parts from a selected List File. One thing to note is that the parameters included in this table will change depending on the active design application. This is controlled by the information that is provided by each application.

Editable columns in the part table

It is possible to process multiple jobs simply by adding more than one list file to the list of parts. If a list file is included in the list that shouldn’t be, click on the Clear button to clear the parts list and then add the appropriate parts to the list.
When ATP parameter files are saved, the part information in this tab is not saved as part of that file. This is because this information represents project-specific information that will change with each job.

Automatic Toolpaths Page 423

Note again that the Process buttons remain visible when this tab is active. If all of the other parameters have been specified correctly, all that is necessary now is to click on the Process <KCDw> button to complete the job. If the ATP parameters have not been defined, the next step is to move on to the Layer Mapping step which is described in the next section.

Selecting Files with No Active Application

In the case where there is not an active design application, part files are selected individually rather than by using a List File. Click on the Select Files tab, and then click on Add to activate an Open Files dialog. Find the DXF files to be processed and select them and click on the Open button and they will be added to the parts list in the ATP.

Select Files Tab

Use these buttons to add and remove DXF files to the list.

Layer Mapping

This dialog is activated when you click on the Add button above. Identify the files to add and click on the Open button.

This is a very important step in the process, and essentially represents the core concept in Automatic Toolpath processing. When design application jobs are created, DXF files are utilized to pass on geometry and other design information. Required machining operations will likely include routing offsets, drills and fills, using a number of different tools and depths.
The geometry in the DXF files is separated onto different layers based on what type of machining will be required. Shapes to be cut out will go on a layer, geometry for dados will go on different layers, and drill points on different layers. This arrangement of geometry on specific layers can be customized to

Page 424 Automatic Toolpaths

match very specific manufacturing methods, but after it has been specified for a given method it likely
won’t change.
The Layer Mapping in EnRoute’s ATP provides a method to synchronize the toolpath creation to match the geometry in the DXF files. As an example, if the rectangle that represents the perimeter of a part is placed on a layer called Cutout, the ATP should be configured to look for the layer Cutout and then to create a routing offset toolpath using the desired EnRoute Strategy. This is where that happens.
First activate the Define Layers tab by clicking on it. The layers table will initially be blank. What is needed is to create a list of layers that corresponds to the layers included in the DXF files of the jobs to be processed. Then Strategies will be assigned to these layers. When the job is processed, these Strategies will be applied to all of the geometry that resides in that layer in each of the DXF files.

Define Layers Tab

Layer Mapping buttons

Define the Layers

The Layer Mapping buttons provide the means to create and edit the layer definitions.

Add Layer – Click this button to add a new blank layer to the list. Remove Layer – Click this button to remove the selected layer. Clear Layers – Click this button to remove all the layers in the list

One method of defining the layers is to add layers one at a time and then edit the Layer Name to match a layer in the DXF files. In order to edit the layer name, just click in the row of the Layer Name column to be edited and type. Continue to add layers and edit them until all of the desired layers have been added.
This can be a complicated process because you may not know all the layer names that are included in the job to be processed. One solution is to import the DXF files into EnRoute in order to find all the layers. A better alternative is to use the ‘Use’ buttons. If a List File has been specified so that a list of parts is active, it is only necessary to click on the Use <KCDw> button to find the layers to map. EnRoute will automatically open each of the part files and extract the layers included and then add

Automatic Toolpaths Page 425

these layers to the layer-mapping table.

Use Active – Click this button to extract all the layers in the active EnRoute drawing.

Use Files – Click this button to extract the layers in the list of individual files that have been selected in the case where no design application is active.

Use <KCDw> - Click this button to extract the layers from the DXF files that represent the parts that have been selected in the parts list. If no parts have been selected, then this button won’t add any new layers.

Click the Use KCDw button to bring in the layers from the active parts list

At this stage, the Strategies have not been mapped to the layers.

Map Strategies

The next step is to select the Strategies to assign to each layer. Remember that strategy templates are saved using the Strategy dialog in EnRoute. Strategy templates can be saved for every type of toolpath that can be created by EnRoute. After a Strategy Template has been saved, it is then available to the ATP to be specified in the ATP Strategy Mapping table.

Click the Save as… button in the Strategy dialog to save the active Strategy as a template. This saved template can then be used by the ATP

Page 426 Automatic Toolpaths

Use the Strategy template dropdown to review the names of the saved strategies, and to select a template to activate.

In the ATP dialog, the saved Strategy templates are selected for mapping to each layer in the list. Both a normal Strategy and a Small Part Strategy may be selected for each mapped layer. The Small Part Strategy will be used for any parts that have a surface area that is less than a threshold defined by the user in the EnRoute Preferences dialog.

In order to select a strategy in a layer, just click on the dropdown arrow on the right side of each strategy cell. This will display a list of all eligible saved strategies. The type of strategy is shown in parentheses next to each strategy name. For example, in the following screen capture, the first strategy in the list is ‘Panel T0375 D075(offset-male)’ which tells us that this is a male routing offset strategy. In this case, the name of the strategy was used to provide some information about the tool and depth, and its name was created to match the name of the layer it is to be assigned to. There are many different strategy naming conventions that can be used, and each user should arrive at a system that works best for their situation.

Both a normal Strategy and a Small Part Strategy may be defined. The Small Part Strategy is utilized for parts that have a surface area below a threshold that is defined by the user. If a Small Part strategy is not defined, then the Strategy is used for all the


Automatic Toolpaths Page 427

Activate the Preferences dialog by clicking Setup and Preferences… Then click on the Initialization tab to show the area threshold for small parts.

After strategies have been mapped to each of the layers, it is necessary to define several additional parameters in order to complete the Layer Mapping task. These include Design Depth/Use Depth, TP, NT, NS and OP. Although the representation of these parameters is a little cryptic, the settings will likely remain the same for most of your jobs.

Additional parameters in addition to the Strategies that must be defined for each mapped layer.

Design Depth/Use Depth – This parameter provides a way to utilize any given Strategy template for more than one cut depth or thickness of material. ‘Design Depth’ refers to the depth that the selected Strategy was configured for.

When Strategy Templates are created, the strategy is specified with a specific depth. If a routing offset depth is set to a depth of 0.50 inches, then this is the depth at which toolpaths will be created when this strategy is applied. If this strategy is used to cut out material that is 0.50 inches thick, then this works great. However, if I also want to use this same strategy to cut out material that is 0.75 inches thick, there could be a problem. The Design Depth parameter helps solve the problem. In this case, I would set Design Depth to 0.50 inches, and click on Use Depth to put a check in the checkbox.
When the DXF geometry is created by the design application, it is typically placed at the depth at which it is intended to cut. Contours that are to be cut at 0.50 inches are placed 0.50 inches below zero in the vertical (Z) axis. If Design Depth is specified, and Use Depth is checked, EnRoute uses the vertical position of the contour to determine whether to automatically adjust the Strategy depth. In our example, if the contour is at -0.50, then no changes are made, but if the contour is at say -0.75, then

Page 428 Automatic Toolpaths

the strategy would be modified to have a depth of 0.75. This means that the same strategy could be assigned to layers that will import geometry at different depths.
Some good examples of this include dado layers that are intended to cut at different depths, and cutout layers that may be used for cutting 0.25, 0.50 and 0.75-inch-thick material. The advantage to this method is that it ultimately requires fewer strategy definitions to accommodate the range of toolpaths that may need to be created on a job.
When Strategy templates are saved, it may be a good practice to include the design depth in the name of the strategy so that it is easy to remember this number as it is utilized in the ATP.

TP – Toolpath. This provides an option for creating toolpaths for the geometry on each layer. Most of the time this parameter should be checked. There may be cases, however, where information on a particular layer should not get toolpaths, but it should be included in the processed files.

NT – Nest Together. This tells the ATP that this layer should be included with the ‘part’ that is defined in the rest of the DXF file. When output from a supported design application is being processed, this parameter should always be selected. There may be certain situations when DXF files that were created some other way are being processed. In these cases, it is possible that several parts may be included in one file, and this is the situation that may work better using the NS (Nest Separate) option.

NS – Nest Separate. This option tells the ATP to treat individual contours as separate parts, and to not treat each DXF file as a complete part. See the discussion for the NT option for the situations when this may be appropriate.

OP – Output. The layer should be included with the part in the toolpath output. This should be checked in virtually all cases. There may be unique situations in which geometry information is included in the part files that should not be included in the output.

Default Strategy

The Default Strategy provides an option for specifying a Strategy to be utilized in case a layer is included in the processed parts that is not included in the layer mapping. It is not necessary to specify the Default Strategy.

Automatic Toolpaths Page 429

Ordering and Nesting

After the layer mapping is complete, then it is necessary to specify how the toolpaths should be ordered, and then how the parts should be nested. This part of the process is virtually the same as the ordering and nesting that is performed within the normal EnRoute output process.
To activate this tab, click on the Ordering and Nesting tab in the ATP dialog.

Ordering Options

The ordering options are the same as within EnRoute. A detailed description of this is included in
Chapter 10. The following provides a description in the context of the ATP.

The Ordering Options provide the means of

specifying the order of the toolpaths when the output

files are created.


The Priority determines the order in which the toolpaths are ordered, using each of the five Priority options. These items may be placed in the desired order by clicking on the item to be moved, and then clicking and dragging on the item to move it.
When the output is created, the toolpaths are ordered working from the bottom item in the list up to the top Priority item. For a given output file, the toolpaths are ordered five times; so, for the list in the dialog above they would be ordered first based on the order of the Layers, and then based on the Pass depths, then based on the sorted Objects, then based on the Strategy Order, and finally based on the Tool Order.
The result of this process is that the toolpaths will always be ordered to match the order of the top Priority item. They will be ordered to match the order of the second Priority item to the extent that it is consistent with the Tool Order, and so on down the Priority list. This means that the top items have the most impact on the order of the toolpaths.
The following simple example illustrates the concept of the Priority Ordering of toolpaths using numbers to represent toolpaths.

Page 430 Automatic Toolpaths

The following numbers are unordered. The numbers aren’t repeated, and

they are either big numbers or small.

5, 8, 3, 9, 2, 7, 14, 6

The numbers are first ordered based on their numeric sequence.

1, 2, 3, 4, 5, 6, 7, 8, 9

Now, the numbers are ordered based on size, with the small numbers first, providing the following final order.

3, 5, 6, 7, 9, 1, 2, 4, 8

You can see that by ordering by numeric sequence first and then size we get a specific order to the numbers. Within each of the two size groups, the numbers are in numeric sequence even though they are not in numeric sequence overall.

In the second option the numbers are first ordered based on their size.

8, 2, 1, 4, 5, 3, 9, 7, 6

Now, the numbers are ordered based on numeric sequence, providing the following final order.

1, 2, 3, 4, 5, 6, 7, 8, 9

You can see that by ordering by size first and then numeric sequence we get an order that is quite different than in the first option even though all we did was switch our ordering priorities.

Tool Order

The Tool Order gives the opportunity to define the order of the tools that are used in the current job. This order is used when the toolpaths are ordered using the Tool priority. EnRoute automatically lists the tools that are utilized in the Strategies included in both the Layer Mapping and the current parts to be processed.

Note that EnRoute checks both the parts in the parts list as well as the Strategies in the layer mapping for the tools. This means that if you have not yet specified any parts to process, there won’t be any tools in this list. As soon as parts are selected to process, the required tools will show up in the tool list.

Tools can be included or excluded from the output by checking or un-checking the Use checkbox for each tool.

Automatic Toolpaths Page 431

Tool Order shows the order of the tools required by the current Layer Mapping and parts list. The tools can be moved in the list to the desired tool output order.

Strategy Order

The Strategy Order is similar to the Tool Order. The Strategy list is populated using the strategies from the layer mapping, for those parts that are included in the parts list. This order is used when the toolpaths are ordered using the Strategy priority. A strategy can be excluded from the output by un - checking the Use checkbox for that strategy.

Strategy Order shows the order of the strategies required by the current Layer Mapping and Parts list. The strategies can be moved in the list to the desired output order.

Sort Method

The Sort Method defines how parts on a sheet will be sorted. This part order is used when the toolpaths
are ordered using the Object priority.

Page 432 Automatic Toolpaths

Sort Method lets you select how the parts on each sheet will be sorted. Typically, you will use the Shortest method, but you may occasionally prefer to sort the parts into Rows or Columns.

Small Parts First – This checkbox lets you ensure that the parts will be sorted so that any parts that are smaller in area than the Small Part threshold will be ordered before the larger parts. This option can be particularly useful if you are using a vacuum system to hold parts down. It allows the small parts to be cut out first, when the vacuum is most capable of holding them down.

Nesting Options

The Nesting Options provide the parameters to specify how the parts should automatically be arranged on the sheets as they are prepared for output. The nesting process attempts to make the most efficient use of the material, minimizing waste.
EnRoute and EnRoute Wood use a true-shape nester, which means that it considers the precise shape of the part instead of treating the part as a rectangle in all cases. The advantage of true-shape nesting is that it can make the best use of the material by arranging parts so that waste is minimized.
Nesting of the parts is a key step, because the nested sheets are the basis for the output files that are created. When the parts are processed, an EnRoute drawing is created that contains layers that represent each of the nested sheets. Each drawing layer corresponds to an output file. In the nested sheet drawing, the layer names correspond to the material that sheet represents.
During the nesting process, the ATP keeps parts that are to be cut from the same material together. This means that if you have a job that includes ¾” melamine, ¼” plywood, and ½” plywood, then all of the ¾” melamine parts will be nested together, all of the ¼” plywood parts will be nested together, and all of the ¾” plywood parts will stay together. EnRoute uses the material names included in the List Files to determine what material each part will be cut from.

Automatic Toolpaths Page 433

Nesting Options provides the parameters for EnRoute’s true- shape nester to arrange parts on the sheets.

Angle Step – These are the angle increments that the nester uses for each part as it works to find the best arrangement of the parts on the sheet. Smaller angles increase the number of options that the nester must consider, so it increases the amount of time to nest each sheet.

When processing files in the ATP, much of the material to be cut has a wood or some other directional surface so often times it is best to set the step angle to 180 degrees. This minimizes the options for the nester to consider, and will help reduce processing time. Even when the material is not grained, experience shows that setting the step angle to some value below 90 degrees most often is not necessary in order to make the best use of the material.

Gap – This is the spacing between the individual parts. The overall size of each part includes the size required by any external toolpaths, so it is often acceptable to set the Gap to a very small value, or even 0.0, in order to maximize material usage.

Margin – This is the spacing from the edge of the sheet of material to the parts nearest the edge. Again, this value may be set to a small value since the boundary of each part includes the toolpath dimension.

Multilayer – This tells EnRoute that it can create new sheet layers in the output drawing as necessary in order to nest all the parts. For example, if there are 50 parts to be cut from ¾” melamine and only

10 parts will fit on each sheet, EnRoute will automatically create the 5 sheet layers in the output drawing
required to nest all the parts. Consecutive sheet layers are named to show how many sheets are required of each material.

Use Holes – This allows the nester to utilize the holes in which to nest parts on a sheet. This option does not typically get used with the files that are most commonly processed in the ATP. The following graphic shows the difference between nesting with and without the Use Holes option checked.

Page 434 Automatic Toolpaths

Use Hole is Unchecked -

The rectangles have an inner

‘hole’ that could potentially be used for cutting parts. If Use Holes is not checked,

then objects are not placed

in these holes.

Use Hole is Checked - In this case you can see that the holes are utilized for

placing objects. The result is that it can be possible to cut the same number of parts by

using less material.

Plate Size

This section tells the ATP what size material is going to be used for cutting the job, and where surface is to be defined.

Plate Size tells the ATP what size material will be used for cutting the parts, and where the surface will be defined on the machine.

Width – This is the X dimension of the material. The units of this dimension match the active units in


Automatic Toolpaths Page 435

Height – This is the Y dimension of the material.

Thickness – This is the default Z dimension of the material. When output is created for the active design application, the plate thickness is automatically adjusted as necessary to match the thickness of the parts on each sheet. If files are being processed with no active design application, or if the active EnRoute drawing is being processed then this thickness is used.

Surface – This is a user preference that may change depending on the machine being used, or the type of material being cut. Typically, the surface is set to the bottom of the plate because then small variances in material thickness do not cause problems when cutting parts out.

Grain Direction – The assumption is that parts coming into the ATP are oriented based on the grain direction in the X direction. If this parameter is set to the Y direction, then parts are automatically rotated by 90 degrees as they are imported from the DXF files.

ATP Setup

The Setup tab contains parameters that determine what type of output files are created when a job is processed. There are three types of output that can be generated, including (1) the machining output files (the g-code files), (2) a printout of each nested sheet that shows what parts are included on each sheet, and (3) label output files that allow labels to be printed for each part.

Output Options

These checkboxes allow you to choose what output you would like to generate.

Create output files – This option creates the machine files that will be sent to the router. The files will be located in the location that is specified in the Output Settings section described below.

When a job is finished processing the ATP provides a message box that lists the output files created.

Page 436 Automatic Toolpaths

Create printout of parts – This option prints an image of each nested sheet, including a text label that identifies each part on the sheet, as well as a title that is the name of the output file that was created. This type of printout makes it much easier to identify individual parts so that they can be organized as they come off the machine after they are cut.

The barcode button to the right of this checkbox allows you to specify a barcode font that will be used to generate a barcode version of the filename of the output file. Some machine manufacturers allow their users to locate and track output files using barcodes and this helps facilitate that option.
The following image shows an example of a printout of a job processed in the ATP.

Create label output – This tells EnRoute to generate label output using the parameters defined in the Label Settings on this dialog. Labels provide a higher level of tracking ability for the parts. This is an option that can be added to the standard EnRoute Wood package that allows you to design and generate individual labels for each part that you process in the ATP. Labels can form a key part of a manufacturing process. EnRoute uses an XML format that makes it easy for design applications to provide a wide range of information to EnRoute that can be passed along to each label. Information about edge banding, customer, finishes, or virtually any other information can be included in labels.

Following is an example label. It was designed to include standard information about the filename, dimensions and material. It also includes a thumbnail view of the nested sheet that shows which part this label is for, along with an arrow that indicates the orientation of the part on the sheet.

Automatic Toolpaths Page 437

Output Settings

These two parameters tell EnRoute where the output files should be placed, and how they should be named. The Output Path button activates a dialog for specifying the path to the output files. This path is displayed to the right of the button.
The Output filename parameter serves as a prefix to the names of the output files. It is a way to define filenames that are easily identifiable. Output files are automatically named using the material name for the parts. If the Output filename parameter is set, then the material name portion of the filename is appended after this parameter.

As an example, if the Output filename parameter was set to ‘Smith01’ and the material it was to be cut using is ‘3/4 Plywood’ then the output filename would be ‘Smith01_3_4 Plywood.cnc’. Notice that the ‘/’ is replaced with ‘_’ since this is not a legal character in a filename. Also, the extension on the filename would be based on the active machine.

The Output Settings parameters allow you to specify where output files are saved, and a prefix to the file names.

Page 438 Automatic Toolpaths

Label Settings

If the labeling option is enabled, these parameters are used to select the size and design of the labels to be printed. Two separate applications are used to define Label Design and Label Format files.

Label Design – This file format uses the XML file format to specify the layout of the labels. The files

have an ‘lds’ extension and are created using EnRoute’s Label Designer™ application.
Label Format File – The label formats specify how labels are arranged on a sheet. Many standard label formats are provided with EnRoute, and new ones are easily created using the Label Maker™ application. The ‘lfc’ file format stores the label format, and is selected with this parameter.

Label Format – When the Label Format file is specified, its individual label formats may be selected using this parameter.

Example Steps to Process Your Files

The previous sections describe each of the steps required to use EnRoute’s Automatic Toolpath feature to process part files. This section provides a brief step-by-step listing of how you would typically proceed through the process. It follows the flowchart described in the ATP Overview presented at the start of this chapter.

Processing a Job Starting from Scratch

These steps assume that you are setting up the ATP from the start, and have not yet performed any
Layer Mapping and have not set any of the other parameters in the ATP.

1. Start EnRoute.


2. Define strategy templates in EnRoute based on the machining operations and tools you typically use.

If you are a new EnRoute user, this will likely take some trial and error on your part to determine the machining operations you will typically use.

3. Set up the EnRoute Tool Library to include the tools you will use with your ATP machining.

EnRoute is supplied with a default tool library that you will likely modify to meet your needs.

4. Configure the Machine Setup parameters in EnRoute so that they match your actual machine configuration.

This will likely include configuring your tool changer and/or drill bank to match your machine configuration.

5. Start the ATP.

You are now ready to set up the ATP.

Automatic Toolpaths Page 439

6. Go to the Setup tab and set the Active Design Application.


7. Go to the tab for the active application (KCDw, etc…) and

select the File List for the job you would like to process.

Prior to this you should have created job output from your design application.

8. Go to the Define Layers tab in order to define the Layer Mapping.

Now we need to set the layers and strategies we will use to process the job.

9. Click on the Use KCDw (or other application) button in order to find what layers are used.

This will extract all of the layer names from the DXF files in the active job so that you don’t have to search them out yourself.

10. Select a Strategy for each of the layers.

These will be used to process the geometry on the corresponding layers in the parts.

11. Select a Small Part Strategy for the cutout layer(s) if that is desired.

Remember that you need to define the small part threshold in EnRoute’s preferences if you are going to use this.

12. Define the Design Depth/Use Depth parameter for each layer.

If you would like EnRoute to automatically adjust toolpath depths based on the geometry depth in the DXF files, define the depth that the strategy was designed for and then check Use Depth.

13. Select TP, NT and OP

for each layer.

These parameters should be checked for virtually all standard applications.

14. Define a Default

Strategy if you want one.

This probably isn’t necessary for standard jobs, and it could

get you in trouble if a surprise layer shows up in a file.

15. Click on the Ordering and Nesting tab


16. Set the Priority order you want to use.

You likely want to have either Tool or Strategy at the top of the Priority list.

17. Define the Tool Order.

EnRoute extracts the tool list based on your Layer Mapping. Generally, move tools used for drilling and fills ahead of tools used for routing offsets.

Page 440 Automatic Toolpaths

18. Define the Strategy


These are the strategies that the Layer Mapping uses. Typically, you want to have the male routing offsets at the end so that objects don’t cut out before they have finished the other operations.

19. Select the Sort Method.

Typically, the Shortest option works fine.

20. Set the Plate Size.

What size material are you going to use? 96x48, 97x 49 etc… If you are processing output from a design application, then the thickness parameter will be adjusted automatically.

21. Set the Surface option.

Do you typically set the machine surface at the top or bottom of your material?

22. Set the Grain Direction.

Typically leave it in the X direction.

23. Set the Nesting Options.

Angle Step = 180 or 90

Multilayer = checked

Use Holes = unchecked

Gap = 0.0 or some small number

Margin = 0.0 or some small number

Position Button = Bottom, Left or Lower Left typically.

24. Click on the Setup tab.


25. Set the Output Options.

Check the appropriate options. If this is the first time through, you may not want to generate any output until you have reviewed a few jobs. Because EnRoute creates an active drawing containing all the nested sheets it is easy to review the results of the processed job without having any other output created. Just scroll through the layers to see the nested sheets.

26. Set the Output Settings.

Tell EnRoute where to send the output.

27. Set the Label Settings.

If you are creating label output, choose a label design and a label format. Remember that labeling is an optional feature.


Before you do any processing, click on the Save button and save all of the setting you have defined. Then when you need to make changes you will only have to change the parameters that need to be modified.

29. Click on the Process

<KCDw> button.

The button will have the name of whichever design application you are using.

30. Click on the Close button and review the results of the job in the active EnRoute Drawing.

You will be prompted to Save Changes. If you click on Yes, then all of the parameters and the list of parts will be retained so that if you get back into the ATP things will be as you left them.

Automatic Toolpaths Page 441

Processing a Job Using a Saved ATP File

This example assumes that you have already defined the job parameters and now need to process a new set of part files. It illustrates that after you have been through the process of mapping the layers and setting the other processing parameters it becomes very quick and easy to process jobs that can contain dozens of parts.

Open the ATP.


Load the List File you want to process.


Load the saved ATP file.


Click on Process <KCDw>.


Review the nested sheets.

Flip through the sheets in the EnRoute drawing to make sure things look correct.

Send the output files to your machine.


Labels in EnRoute

EnRoute’s Automatic Toolpath processing includes the ability to produce labels that can be printed out for each of the parts that is processed. In addition to EnRoute, there are three applications that are utilized to design, format, and then print the labels. Following is a brief description of each application, followed by a more detail explanation of using each.

Label Designer

This application provides tools for creating custom label designs. Size, layout, information, and layout are created and saved, and can then be specified in EnRoute as the design to be utilized when processing a job.

Label designs are stored in individual design files, typically in the \EnRoute6\AutoTP\Labels folder. These files have a .lds extension. They are XML formatted files.

Label Maker

This application lets you design the format of the labels on the sheet on which they are printed. This can be very simple if the labels will be printed on a dedicated label printer. It can also

be more involved if you are using labels that are formatted on a larger sheet of


Label formats are stored in a file named LabelFormatCollection.lfc created by LabelMaker. You also use it to choose the active printer for printing labels.

Label Printer

This application provides another method of printing labels. After opening a label output file, it provides a preview

Label Printer uses the same active printer as defined by Label Maker

Page 442 Automatic Toolpaths

of each label, and allows you to choose which labels you want to print, and even how the labels are laid out on the
sheets to be printed.

Label Designer

The Label Designer application allows you to design custom labels for use with the ATP. Designs can include standard part information that is produced by EnRoute as jobs are processed. They can also include custom information that is passed to EnRoute by design applications that produce the part files.
When EnRoute processes a job, the label design is used to produce the label output files that represent each of the parts in the processed job.

Designing a Label

The process of designing a label includes first defining the label size, and then position text, graphics, and possibly bar codes on the label. The text and graphics can be specific words and graphics, or they can be “placeholders” that define what data will go on the label that will be unique for each label. The following steps provide a description of creating a label design from the beginning.

1. Open the Label Designer. It can easily be accessed from the flyout toolbar that is activated in EnRoute by clicking and holding the ATP icon.

2. Click File and New to create a new label. The Label Design Properties dialog comes up allowing you to define the size of the new label, along with a name.

Automatic Toolpaths Page 443

3. The blank label design is shown. The interface is similar to EnRoute’s but includes a set of object placement types that are specific to labels.

4. Set the units for the label by clicking on the View and Units menu items.

5. Start the design process by choosing to place Text, Barcode, or a Picture. The default mode is the selection mode, which is the arrow. This allows you to select objects for editing and moving.

6. Click the Text tool and then click and drag a rectangle on the label to define where the text object should be placed. Don’t worry too much about where it goes because you will likely scale and move it

to put it in place.


Page 444 Automatic Toolpaths

7. The Object Properties dialog is activated. This allows you to define precise size and placement of the object, along with its attributes and what data it might utilize.

8. The Attributes tab provides the chance to choose font and alignment properties, as well as define the text that goes in the text object. The text may be the actual literal text the label should have, such as a company name, or it might just be placeholder text that will be replaced

each time the label is created.

9. The Data tab allows you to make the decision about whether the text object should be interpreted as a literal label, or whether it serves as a placeholder for data that will be specific for individual parts. In the case of this example, you can choose to have the text include the literal phrase “Part Name”, or you can have it hold the place for the actual part name that will come from likely come from the design application list file.

Automatic Toolpaths Page 445

10. If you choose to use the Text as a placeholder, click the check box to indicate this. Then choose the data field you want to use from the list in the combo box.

11. By default, the items in this list are the standard data items created by EnRoute when it processes parts. It is possible to modify this list to include additional data that can be passed from design applications to EnRoute.

This is a slightly more involved process that will likely require assistance from

the EnRoute team.

12. Next you can choose to create a Picture for your label. This can be an image such as a company logo, or it can be picture data, such as a thumbnail image of the nested sheet. First select the Picture Tool…

13. …Then draw a rectangle on the label. This indicates where the picture will be located. As with the text, it is always editable so the size and location can be


Page 446 Automatic Toolpaths

14. The Layout tab lets you define size and location.

The Attributes tab gives the

option to choose a specific bitmap image to include. This is how you might

choose to include a company logo on each label. Most often, it’s not necessary to choose a file because the

picture will serve as a placeholder for a graphic that will be generated when the parts are processed by


15. As with the text object, the Data tab allows you to define the picture as a placeholder for an image that will be created with the processing. By default, there are three image types that are generated by EnRoute. These include a Thumbnail

of the nested sheet, a Part

Preview of the individual part, and a Compass, which

is an arrow that indicates the

orientation of the part as nested on the sheet.

16. Barcode object types are placed in much the same way as text and pictures. The Attributes tab lets you choose the encoding method, and that Data tab shows the data types that are compatible with a

barcode encoding. Typically, part number or part name

are used here.

Automatic Toolpaths Page 447

17. After placing an object, it can be easily edited by just double-clicking on the object. This activates the Object Properties menu so that you can adjust size and placement, or adjust the choices for data to be used.


18. Label Designer also allows you to Cut, Copy and Paste objects, as well as Align objects on the label.

19. After the design has been completed, click on

File\Save or File\Save As to

save the label design to a file. Typically, you will give it a descriptive name so that it is easy to find when it is time to use it.

EnRoute comes with several label designs that can be used as-is, or modified to fit your needs.

20. In EnRoute, the label design is specified in the ATP dialog, on the Setup tab. It is available the next time EnRoute is started after the label file has been saved to the EnRoute6\AutoTP\Labels folder.

Page 448 Automatic Toolpaths

Label Maker

The Label Maker application provides three main functions,

 It is used to define Label Formats, which specify how labels are arranged on a sheet of labels for printing. For dedicated label printers, this might typically be one label per sheet, but it can also be several labels on a standard letter-sized sheet.

 It is used to select the active printer for label printing – for both Label Maker and Label


 It is used to send label output that is created by EnRoute to the printer. The following steps show how the label formats are defined.

1. Open the Label Maker. It can easily be accessed from the flyout toolbar that is activated in EnRoute by clicking and holding the ATP icon.

2. Label Maker has a simple- looking interface.

Automatic Toolpaths Page 449

3. Choose Settings\Label to activate the Label Setup dialog.

4. In the Label Design tab, you can define the units for the format, as well as the Label Design that should be referenced.

5. The Label Format tab allows you to specify how the labels will be arranged on a sheet of labels.

If you are printing using a dedicated label printer, you might likely configure it to include only one label. On the other hand, if you are printing a sheet of labels, as shown in this image, you can define the number of columns and rows of labels, along with margins and offsets. Information from the label manufacturer will provide details.

After defining parameters, click on the Save As button to save the format to be called by EnRoute. This information is included in the label output created by EnRoute. When finished, click OK.

Page 450 Automatic Toolpaths

6. Click on Settings\Printer to activate the Printer Setup dialog. This allows you to choose the active printer to use when printing from within Label Maker and also from within Label Printer.

When done, click OK.

7. After defining the label format, in EnRoute you can choose that label format to be utilized

when the ATP job is processed.

To create labels…

 Make sure Create label output is checked

 Select a Label Design

 Select the


 Select a Label Format Name

8. When the job is processed, the label output will be created a placed in the output folder.

Automatic Toolpaths Page 451

9. After label output has been created by EnRoute, Label Maker is also used to send the output to the selected printer. To print a job, select File\Open
and then navigate to the desired output folder and select the desired .ljd output file.

Label Printer

The Label Printer application was created as a way to better visualize labels, and to provide additional control over label printing. It uses the Label Format that is defined in the label output file, and the active printer as selected using Label Maker.

Page 452 Automatic Toolpaths

Label Printer provides the following unique features,

 Its interface allows access to multiple label output files at one time. If you process a job that creates several sheets of labels, you can page through each of the output files.

 It shows the layout of the parts on the nested sheet, with the ability to interactively select which labels are to be printed.

 It can show a preview of individual labels as a way of checking to make sure they are formatted correctly.

 It allows you to choose which labels are to be printed. If you need to reprint one or two labels from a nested sheet, this can be very handy.

 It provides a preview of how the labels will be printed on the sheet of labels.

 It allows you to move label positions around. If you have a partial sheet of blank labels this can also help you be more efficient.

After you are familiar with Label Printer, it is simple and efficient to use. Select the job and output file, select which labels to print, and send them to your printer. At the same time, it provides nice flexibility and a good way to review labels before you print them.
Here is a table that walks through the key features.

1. Open Label Printer. It can easily be accessed from the flyout toolbar that is activated in EnRoute by clicking and holding the ATP icon.

2. Click on the Open Job File button. Navigate to the folder containing the label output (.ljd files) that you want to print. Select a file.

3. The Pic filepath should be defined correctly after you have selected the label file. It is either that same folder, or a folder called “pics” that will be a subfolder of the output folder.


4. Layout Rotation is a panel that will likely be collapsed. You can click in the toolbar to expand this panel. It gives the ability to rotate the display of the sheet thumbnail in 90-

Automatic Toolpaths Page 453

degree increments. This is typically not needed.


5. The sheet layout shows the actual position of the parts on the nested sheet. Each part will typically have a label icon located at the center of the part. The following colors have meaning,

 Red – The label is not selected for printing.

 Yellow – The label is selected for printing.

 Green – The cursor is hovering over the label icon which activates the preview of the label in the panel below.

6. Labels can be selected for printing either by clicking on the label icon to toggle its print status, or by clicking on the Select All button at the bottom of the dialog. Click on Select None to un-select all of the labels for printing.

7. When you hover the mouse over a label icon, a preview of the label is shown in the Label Information section of the dialog. It includes a preview of the label, along with a thumbnail of the part itself.

8. If at least one label is selected to print, the Print Selected button will be enabled. When you are ready to print, click this button.


Page 454 Automatic Toolpaths

9. The Labels Layout screen provides,

 A preview of the label sheets as they will be printed.

 You can click and drag individual labels to change their position on the sheet.

 Move a label by clicking to select it and then clicking on one of the four move arrows. If there is more than one sheet, then it is possible to

move a label from one sheet to the next using these buttons.
 If there is more than one sheet of labels, click on the Sheet arrows to move between sheets.
 When you are satisfied with the layout, click Accept to send the output to the active printer.

Automatic Toolpaths Page 455

Page 456 Automatic Toolpaths

23.Keyboard Shortcuts

Bump by Bump


Arrow Keys



Bump By Display


Shift + Arrow Key


Ctrl+ Shift + Z


Ctrl + C


Ctrl + R


Ctrl + X

Shortcut Menu

Right Click

Define Layers



Shift + F7

Define Plate Panels

Ctrl + Alt + P


Ctrl + S




Shift + F6


Alt +X

Select All

Ctrl +A


Ctrl + G

Simulate 2D




Tool Library


Machine Drivers Setup



Ctrl + Z

Material Library



Shift + F8


Ctrl + U


Shift + F5

View Toolpath




Ctrl + N

Zoom In

Ctrl + I


Ctrl +O

Zoom Out

Ctrl + K


Ctrl + V

Zoom Plate

Ctrl + P

Perspective / Top View




Precision Input Center



Keyboard Shortcuts Page 457

Page 458 Keyboard Shortcuts


2D output simulation


ordering and nesting


3D Engrave


output settings


square corners




3D Meshes




apply meshes to relief


Bezier curves


create mesh with EnRoute tools


converting to arcs






import 3D mesh objects








using a mask




3D Sufaces








3D Surfaces Toolbar




3D Toolpaths 163, 229, 391, 401

3D toolpath example 397

displaying 26

inserting 198

Index Page 459

Contour Editing Toolbar




Contour loop indicators


spindle speed








Cutting order




Daisy Chain Toolpaths







104, 106







merging open contours


Deleting Contours


reverse open contour


Depth of cut

155, 160, 165, 171



Depth of toolpaths






Convert Curves to Arcs








array copy tool




copy around and arc




copy contours




path copy




Corner tags






Dimension Toolbar


corner tags





104, 106

angle dimension tool




diameter dimension tool


Create Rendered View


leader dimension tool


Create Shelf Components


radius dimension tool


Creating new files


single dimension tool




Direction arrows on toolpaths


cut contours


Distort Contours

97, 133

Cut by Line Tool


Draft Angle


Cut Definitions




offset from surface






Draw Lines Toolbar



160, 170

Drill bank





211, 215

cut parameters


Drill Toolbar




Drill Tools




creating drill circles


entry/exit points


creating drill points


hatch fill


creating drill points along a countour


island fill


creating drill points in center of contours


open contour offset


drill aray templates




drill arrays


cut templates

154, 164

drill circles template


determining cutting order


drill cut parameters




drill points along a contour template




drive corner templates


entry/exit parameters


Driver Setup


fill 170

fine 170 passes 161 plunge rate 162 rough 160

Dwell 162, 212

Edit Contours Toolbar 47

Edit relief

fade 388 shrink 388

Page 460 Index

Edit Relief

build parameter 389 parameters 387

Edit relief toolbar 387


entry/exit points 195

Editing Points 95 arc 96

bezier curve 96

insert corner tool 97 line segment 95

smooth approximation tool 97


by corners 77 by major and minor axis 77

by, height and width 77

Engrave Toolpath 188

3D engrave strategy 163 cut parameters 190

Entry/exit parameters 163

Entry/Exit Points 195 editing 195 editing cut parameters 196

Entry/exit positions

displaying 26

Exiting the software 30

Explode Selected Contours 109

Exporting a design 64

Extend/Trim Toolbar 47

Extending Contours

apparent intersection 102 precise length 101

to boundaries 101

Extrude 261 extrude dialog 262 extrude example 266

mesh parameters 265 profile placement 264 rotation parameter 264 scale and roatation 263

Extrusions Toolbar 42

Faceted 302

Fade 388

Feed rates 212

File Toolbar 31


creating 57 exporting 64

importing 63

Fill cut 170

Fill Toolbar 45


multiple fillet 106 single fillet 106

Filleting contours 104, 106

Fine Cut 170

Flyout Menus 10

Fractions, converting 155

Generating Output 222

Geometry Creation Wizard 46, 86


grouping contours 121 ungrouping 121

Guidelines 14 creating 14, 15 deleting 15 hiding 16

locking 16 moving 15 rotating 16

Hatch Fill Toolpaths 169

hatch angle 173 hatch vs. island fill 174 overlap 173 template 172

Height Control Curve 256

Help 21

Hexagons See polygons

Holes 119

Import a Design 63

Influence Line 256

Inlay 156, 174 inlay gap 156

Installation 5 hardware key 5

Island Fill Toolpaths 173 corner tags 176 hatch vs. island fill 174

inlay 174 optimization 175 template 176

Jigsaw tool 141

Kerf Compensation 167

Layers 18 changing a contours layer 20 layers dialog 19

Libraries Toolbar 33


drawing 67 editing 95

trimming 102

Machine drivers

active drivers 213 selecting 223

Index Page 461

Mask 333

Material Library 216

Measure 65

Merge 109 merge contours 120 merge selection 109 merge tolerance 109 merging open contours 109


apply mesh to relief 302 create a mesh from a relief 322

create surface 250 extrude mesh example 268 spin example 259 sweep two rails mesh example 276

unwrap mesh 307

Mesh Toolbar 43

Mirroring a Contour 135 interactively 135

mirror horizontal 136 mirror vertical 137

Miter 282

Modify Relief Toolbar 43

Move Objects

move tool 125 moving interactively 122 moving with precision input center 123


bridges 198


arc copy 112 array copy 111

copy around an arc 112

path copy 114

Multiple Fillet 106

Nest Toolbar 45

Nest Tools

block nester 144 dynamic nest tool 152 nest objects tool 143

shape nester 143

New files 57

Nose cone optimization 175

Object Edit Toolbar 35

Octagons See polygons Offset Contours 107 partial offset 108

Offset from surface 393

Offset Toolbar 48

Open contour offset

no 3D toolpaths 167 relief 166

Open Contour Offset Toolpaths 164

Opening a File 62

Ordering options 223

Ordering toolpaths 205, 207, 209, 413


2D simulation 335 output parameters 226

to a file 227

Output Toolbar 34

Overlap 173, 396

Passes 161

Paste 32 paste contours 119

Path Copy 114

Pentagons See polygons

Plan 153 editing 194 plan templates 154 templates 195

Plate 57 automatic fit 58

Creating Plate from Selected Contour 59 displaying 25

Plate Panels 60

Plunge 212

Plunge rate 162


editing 95

Polyarc 67 constructing a line segment 68 construction and arc segment 68


drawing 81

Popup menu 26

Precision Input Center 12

Preferences 21 dimensions tab 27

display tab 24

general tab 22 grid tab 25

initialization tab 23 ordering tab 28

relief tab 27

start points 27 unit tab 25

view setup tab 25

Primitives 294

Print 64

Priority 224

Project Toolpath 202

Pyramid Toolpaths 191 cut parameters 193

Page 462 Index





Radiused Corners

104, 106



Rapid Picture Tool




Rapid Texture




continuous panels






smoothing reliefs


rapid texture dialog


spin tool


Seed Contour


sweep two rails


Texture Examples


wizard prompts




Relief Edit Tools


drawing by corners


Relief Toolbar


drawing by dimensions





18, 32

using bitmaps




Rendered View of Toolpaths




Return height


angles for revolution


Reverse open Contours


application method






Angles for Revolution


merge highest


revolve dialog


merge lowest


revolve example




revolve tool




wizard prompts


apply bitmap example


Right-click menu


chamfer tool




clearing reliefs


rotate interactively


combine reliefs


rotate tool




rotate with precision input center


delete relief objects


Routing Offset Toolbar


extract relief slices


Routing Offset Toolpaths


extrude tool




fit relief to plate








merge reliefs




mesh paramters


reference line




scale tool


modifying and combining


scale with precision input center


moving reliefs


scaling interactively


offset relief surface


scaling line




scaling objects


constant height


Scale and Rotation


limit to height


Scale Toolbar




Scaling Reliefs


scale to height


Screen refresh


relief dialog example


Scroll bars


relief parameters


Setting the Toolpath Order




Settings Toolbar












Simulate 2D




Simulating Output


revolve example


Simulate 2D




Simulate 3D


Index Page 463

Simulate Ortho 206

Single Fillet 106

Sketch 72

Slice Mesh

Slice Mesh Example 297

Slice Meshes

Slice Meshes Dialog 296

Slicing Meshes 296

Slot cuts

templates 187

Slot Toolpaths 187

Smooth 302

Snap 13 snap to center of arc 13 snap to endpoint 13

snap to grid 13 snap to guideline 13 snap to intersection 13 snap to midpoint 13 snap to nearby contour 13 snap to perpendicular point 13 snap to tangent point 14

Snaps Toolbar 39

Snapshot 65

Sort method 226

Spin 251 height control curve 256

influence line 256 mesh surface example 259 spin angles 253 spin dialog 252

spin example 257 width control curve 257 wizard prompts 255

Spindle speed 162, 212

Spiral Fill Toolpaths 176

Stacks 254

Stars See polygons

Start points

displaying 26

Status Line 11

Step Rough 394


adding 195 editing 194

removing 195

strategy templates 154, 166

Strategy 153

Strategy order 226

Support Services 6

Sweep Two Rails 270 sweep two rails dialog 271

sweep two rails example 274

Symmetric Parametric Textures 349

Symmetric Parametric Textures Toolbar 50

Templates 62 cut templates 154, 164 drill array templates 181 drill circle templates 180 drill corner templates 185 drill point templates 179 drill points along a contour 184 island fill template 176 open contour offset templates 166 plan templates 154, 195 plate templates 62 pyramid templates 193 routing offset templates 158 slot cut templates 187 strategy templates 154

Text 82 convert text objects to curves 85

editing text objects 84

Text Toolbar 48

Texture Tools 337 images of 19 types 339

parameter dialog 346

symmetric textures 349 texture dialog 344

Textures Toolbar 48

Tool changer

configuring 211, 214

Tool library 217 custom tool library 219

Tool order 226

Toolbars 10

Toolpath order 226

Toolpaths 153 cuts 154

direction arrows 26

displaying 26 editing groups 194

final depth 26 group plan 153

ordering 205, 207, 209, 413

plan 153 editing 194

toolpath groups 153

toolpath strategy 153 toolpath width 26

Toolpaths Toolbar 36

Triangles See polygons Trimming contours 102 precise length 103

Page 464 Index

to boundaries


jigsaw weld



18, 32

weld common




weld joined



11, 212

weld subtract


Unwrapping Meshes


Width Control Curve


Using a Mask


Width of cuts


Vectorize Bitmap


Width of toolpaths



10, 417



Weld Toolbar


Zoom commands


Welding Contours


Zoom Toolbar


cut by line



Index Page 465