How to Create a Toolpath Pattern - Array

Introduction

This tutorial explains how to create a toolpath pattern using the Array option. The example provided shows how to pattern an individual feature and how to pattern multiple features together using a single toolpath pattern.

Example Part

The part file for this tutorial is available for download at: http://www.bobcad.com/helpfiles. If you are connected to the Internet, you can click the link provided to download and save the Toolpath Pattern Array Example 1 SLDPRT.zip file. After extracting the zip file, you can then open the example file to use with this tutorial. In the example file provided, the stock and Machine Setup are already defined for the part.

 

Part 1) Pattern the First Feature

In the example file provided, two 2 Axis features with pocket and profile operations are already created. The following steps are used to pattern each feature.

 

1. In the Property Manager, click the CAM Tree tab.
   
   

2. Under Machine Setup, right-click 1st Pocket and click Add Toolpath Pattern.

 

The feature being patterned is shown next for reference.

 

 

3. In the Toolpath Pattern dialog box, with Array selected, click Next>>.

 

4. In the X Direction group, in the Distance box, type 5.250.

 

This defines the distance between each feature along the X-axis of the machining origin (coordinate system).

 

The following image shows the distance measured from the center of each pocket. You can use any reference point that you have to measure the distance, as long as the same reference point is used in each pocket.

 

 

5. In the Copies box, type 2.

 

This creates two copies of the feature along the X-axis.

 

 

6. In the Y Direction box, type 3.375.

 

This defines the distance between each feature along the Y-axis of the machining origin (coordinate system).

 

The following image shows the distance measured using the center of each pocket.

 

 

7. In the Copies box, type 2.

 

This creates two copies of the feature along the Y-axis.

 

 

8. To compute the toolpath pattern, click OK.

 

 

Because 2 copies are made along the X-axis and 2 copies are made along the Y-axis, there are a total of 9 pockets created (including the original feature).

Part 2) Pattern the Second Feature

1. To hide the first feature and the toolpath pattern, in the CAM Tree, right-click 1st Pocket, and click Blank/Unblank Toolpath.

 

2. Right-click 2nd Pocket and click Add Toolpath Pattern.

 

The feature being patterned is shown next for reference.

 

 

3. With Array selected, click Next>>.
   
   

4. In the X Direction group, in the Distance box, type 5.250.
   
   In the Copies box, type 2.
   
   

5. In the Y Direction box, type 3.375.
   
   In the Copies box, type 2.
   
   

6. Click OK.

 

Part 3) Modify a Patterned Feature

The last pocket feature contains a single-depth cut. The next part is to add multiple depths to the feature. After modifying the feature, you can see that the toolpath pattern is automatically updated to include the results.

 

1. In the CAM Tree, right-click 2nd Pocket, and click Edit.
   
   

2. On the left side of the dialog box, under Pocket, click Parameters.
   
   

3. In the Depth group, click Multiple Steps.
   
   

4. Click Defined Depths.
   
   

5. In the Depth of Cut box, type 0.250.
   
   

6. Click Compute.

 

 

You can see that not only are the changes added to the feature, but they are also added to the pattern.

Part 4) Add a Hole Feature and Select Geometry

At this point in the example, all of pocketing for this part has been accomplished using two features and two toolpath patterns. The next part is to drill the four holes in each pocket.

 

1. In the CAM Tree, right-click Machine Setup, and click Mill Drill Hole.
   
   The Mill Hole Wizard displays.
   
   

2. Under Geometry Selection, click Select Geometry.
   
   In the Hole Selection Manager, under Point and Arc Usage, the default can be left as Ignore Z.
   
   

3. Click to select each of the cylindrical surfaces of the holes.
   
   
   
   

4. To confirm the selection, click .
   
   The Mill Hole Wizard returns.
   
   

5. In the Geometry Parameters group, notice that the Diameter is automatically set.
   
   Click to clear the Through Hole check box. These holes are blind holes meaning they do not go through the entire part.
   
   

6. Click Next>>.
   

Part 5) Define the Hole Feature Parameters

Important: Because we cleared the Through Hole check box, the tip of the tool will extend past the bottom of the part enough so the full diameter of the tool reaches the specified depth. With Through Hole selected, the tool tip will go far enough past the defined depth that the diameter reaches past the defined depth in the amount defined in the Cutting Conditions Parameters dialog by the Length Through Cut value.

 

1. Notice under Hole Groups, that the Top of Feature is automatically set based on the position of the top edge of the surfaces we selected (-0.375).

 

Note:
• Had the top edge of the surface been selected as geometry for the feature, we could select Use As Top for the selection in the Point and Arc Usage group. The Top of Feature would then be set automatically while the Feature depth would need to be set manually.
• Had the bottom edge been selected, we could select Use As Bottom to set depth automatically and then manually set the Top of Feature.

 

Click Next>>.

 

2. In the Machining Strategy, select the Hole operation template.
   
   The Current Operations list contains one center drill operation and one drill operation.
   
   

3. The operations for the feature are defined, click Next>>.
   
   We use all of the automatically generated drilling operation tools and settings for this example.
   
   

4. At the bottom of the dialog box, click Compute.
   
   
   
   The Mill Hole feature is now complete for the first pocket. The next step is to pattern this feature to handle the drilling for the entire part.

Part 6) Pattern All Features in the Machine Setup

To review what has been done thus far, you have patterned two separate pocket features using two separate toolpath patterns. You have also created a Hole feature to complete the machining of the example part. All of the currently defined operations are shown next for reference.

 

 

At this point, you are ready to add a toolpath pattern to the Hole feature. While you could simply add another pattern as shown earlier in this example, there is another way to pattern multiple features. This part of the example shows how to create a pattern that is applied to all of the features contained in a Machine Setup.

 

1. In the CAM Tree, below 1st Pocket, right-click Toolpath Pattern, and click Delete.
   
   

2. Click Yesto confirm.
   
   

3. Below 2nd Pocket, delete this Toolpath Pattern as well.
   
   These have been deleted so a single toolpath pattern can be created to handle all features.
   
   

4. Right-click Machine Setup, point to Additional Functions, and click Add Toolpath Pattern.
   
   

5. In the Toolpath Pattern dialog box, with Array selected, click Next>>.
   
   

   1. Set the X DirectionDistance value to 5.250.
      
      

   2. In the Copies box, type 2.
      
      

   3. Set the Y DirectionDistance value to 3.375.
      
      

   4. In the Copies box, type 2.
      
      

   5. Click OK.
      
      

All features in the Machine Setup are included in the pattern.

To show the hidden feature, right-click 1st Pocket and click Blank/Unblank Toolpath.

Part 7) Simulate the Program

1. To simulate the program right-click Milling Job, and click Simulation.

 

 To learn more about simulation, view Getting Started with Simulation.

 

The resulting stock model is shown next.

 

 

2. To close the simulation, click (Exit Simulation).

 

 

This concludes the tutorial.

Related Topics

Toolpath Patterns