How to Create Indexing Programs

Introduction

There are two methods that can be used to create programs with indexing.The first method uses Index Systems that are added to the CAM Tree.Thismethod allows you to select geometry or UCS planes as the indexing plane.This is typically used with solid models and it is useful when the indexangles are not known.When using this method, you can view the part indexingto the proper location in simulation.This method is explained first.

Note: Indexingis only available with the 4 Axis Standard and greater modules.

Example File

The BobCAD part file for this tutorial is available here C:\BobCAD-CAM Data\*Current Version*\Examples\Indexing.bbcd.In this example, you learn how create an indexed part.

Create Indexing Programs Using Index Systems

The Machine Setup in the CAM Tree is used to define the machining origin(work offset) of the part on the machine.To use Index Systems, you mustfirst create stock for the part and define the Machine Setup.You thenadd an Index System to the Machine Setup in the CAM Tree.After addingan Index System, you select a plane to define the indexing position.Oncethe indexing plane is defined, milling features are added to the IndexSystem.This tutorial is designed to explain the setup process.The partfor this example is shown next.

Note: Indexing can also be accomplished using the Output Rotary Angle parameterthat is available in the Posting page of the Milling Wizards.For thismethod, you use the Rotation Angle parameter to create the proper indexingin the posted program.The indexing of the part is not visible in simulation,it is only output in the posted NC program.

Part 1) Create the Job

1. Create a New Job by either: 
   
   
   1. In the CAM Job group, of the CAM ribbon, click New Job.
      
      
   2. In the quick access toolbar of the CAM Tree Manager, click New Job.
      
      
   3. In the CAM Tree Manager, right-click CAM Defaults, and select New Job.

Part 2) Select the Job Type and Machine

1. With the Job Type set to the default Milling, click the down arrow under the Machine, and select the BC_4x_Mill.

Part 3) Create Stock for the Part

1. In the Machining Job dialog, click Stock Wizard.
   
   The Workpiece dialog appears, allowing you to select the workpiece to appear in the simulation.
   
   This can be ignored, or the desired solid can be selected in the graphics area.
   
   
2. Whether a workpiece has been selected or not, click >> to move to the Stock Definition dialog.
   
   
   
   The default Rectangular stock appears around the model.
   
   
3. Click in the Stock Type section to set the stock to a cylindrical shape.

Part 4) Define the Machine Setup for the Part

In the Machine Setup dialog box, the stock is outlined withentities that are automatically created to help you select the machiningorigin.

1. In the Coordinate Systemgroup, click in the Origin list to give it focus, and clickon the back end of the edge of model as seen in the image below.
   
   
   
   

2. The default ClearancePlane value is used.
   

   Note: The value set here is used for all features added to this MachineSetup in the CAM Tree.

   The next step is to define the distance from the machine zero to themachining origin of the part, which is set on the top of the cylindricalstock, but for this example, we will skip that until later.
   
   

4. The Machine Setup for the part is now defined.To finish, clickOK.

Tip: To hidethe stock from view while working, right-click Stock, and click Blank/Unblank.

Part 5) Add an Index System to the Machine Setup

Important: Beforeadding milling features to an index system, you must define the indexingplane as explained in this example.When adding milling features usingIndex Systems, you must right-click the IndexSystem and not the Machine Setup.This is the only way to have the proper angles set by the software.(Ifyou add a milling feature using the Machine Setup, the feature is notadded to the Index System.)

1. To add an Index System, in the CAMTree, right-click Machine Setup, point to Additional Functions, and clickAdd Index.
   
   The Index System Selection dialog appears in the Data Entry Manager.
   
   

Tip: If you do not have a planar face or surfaceto select, you can select a UCS, in the Index System Select dialog box,to set the index plane.

3. Click the face with the drill holes.
   
   
   
   

4. The face is added to the Selected Geometry list, and a preview of the index system is displayed.
   
   
5. Click OK.
   
   The index system is set, and you are ready to add milling features.
   

Part 6) Feature Setup

1. in the CAMTree, right-click Index System, and select Mill Drill Hole.
   
   The Mill Hole Wizard appears.
   
   
2. Click Select Geometry.
   
   The Mill Hole Wizard disappears, and the geometry picking dialog appears.
   
   
3. In the Data Entry Manager, the Selected Geometry list automatically has focus to allow you to select geometry.
   
   Select the inner surfaces of the two holes.
   
   
   
   Each is added to the Select Geometry list.
   
   
4. Click OK.
   
   The Mill Hole Wizard reappears.
   

Note: By selecting the surfaces and not the surface edge, the hole feature can recognize the proper depth to use for the holes.

5. Click Next>> twice to go to the Machining Strategy page.
   
   
6. Select the Hole Template.
   
   
7. Since we are not concerned with drill settings in this example, click Compute.
   
   
   
   The Mill Hole Wizard disappears, and we can see proper toolpath on our part.
   

Part 7) Add another Index System to the Machine Setup

1. To add an Index System, in the CAMTree, right-click Machine Setup, point to Additional Functions, and clickAdd Index.
   
   The Index System Selection dialog appears in the Data Entry Manager.
   
   
2. Click the face with the pocket.
   
   
   
   
3. The face is added to the Selected Geometry list, and a preview of the index system is displayed.
   
   
4. Click OK.
   
   The index system is set, and you are ready to add milling features.
   
   

To learn how to use toolpath patterns with index systems for repetitivetasks, view Howto Create a Toolpath Pattern - 3D Rotate.

Part 8) Feature Setup

1. in the CAMTree, right-click the second Index System, and select Mill 2 Axis.
   
   The Mill 2 Axis Wizard appears.
   
   
2. Click Select Geometry.
   
   The Mill 2 Axis Wizard disappears, and the index system appears on the part.
   
   
   
   
3. In the Data Entry Manager, the Selected Geometry list automatically has focus to allow you to select geometry.
   
   Select the bottom of the pocket.
   
   
   
   The face is added to the Select Geometry list, and the feature preview appears.
   
   
4. In the Data Entry Manager, in the Feature Parameters group, click in the Pick Top list of the Top of Feature group to give it focus.
   
   
5. Click the top edge of the model to set that as our top of feature.
   
   
   
   The feature preview updates.
   
   
   
   
6. In the Data Entry Manager, in the Feature Parameters group, click in the Pick Bottom list of the Top of Feature group to give it focus.
   
   Click the bottom edge of the pocket.
   
   
   
   The point is added to the Pick Bottom list.
   
   
7. Click OK.
   
   The Mill 2 Axis Wizard reappears.
   
   
8. In the tree on the left of the wizard, click Machining Strategy to jump to that page.
   
   
9. In the Template list, select Pocketing.
   
   
10. In the Current Operations list, select Profile Finish to highlight it, and click Delete.
    
    The operation is removed from the current operations list.
    
    
11. In the tree on the left of the wizard, click Rough to jump to the tool page.
    
    
12. Update the Diameter value to 0.2500.
    
    
13. In the tree on the left, click Parameters.
    
    
14. Update the Side Allowance to 0.0000.
    
    
15. Click Compute.
    
    The Mill 2 Axis Wizard disappears and the toolpath is visible.
    
    
    

Part 9) Simulate

In this portion of the example we show the importance of setting the Work Offset in the Machine Setup.If you have Machine Simulation Pro, follow along.If not, there is no need to simulate.

1. In the quick access toolbar of the CAM Tree Manager, click Simulate to launch the simulation.
   
   The simulation launches.
   
   
2. In the Simulation group of the Simulation tab, ensure the Machine option is selected.
   
   
3. Notice the components colored in red signifying a collision.
   
   
   
   By zooming in, you can see the stock is completely inside of the chuck, and that is not centered.
   
   This is because the machine zero we set at the beginning of the job will be placed at machine zero.To offset this, we must adjust our work offset.
   
   
4. In the Simulation group of the Milling ribbon, click Exit Simulation to exit the simulation.
   
   

Part 10) Adjusting the Work Offset

1. In the CAMTree, right-click Machine Setup, and select Edit.
   
   The Machine Setup dialog launches in the Data Entry Manager.
   
   
2. In the Layers Manager, right-click the Dimensions layer, and select Show Layer.
   
   The dimensions become visible.
   
   
3. Click Work Offset at the bottom of the Data Entry Manager.
   
   The Work Offset dialog launches.
   
   We want to enter the values that show how the Machine Setup has moved from the WCS, which is the center of rotation on our machines.
   
   
   
   
4. We can see in the dimensions, we need to adjust the Y, and Z values to center the stock in the chuck, and we need to add a negative X value to pull it out of the chuck.
   
   In the Work Offset dialog, change the values to: 
   
   X = -7.000
   Y = -0.500
   Z = 0.866
   

Note: Notice all these values are referencing the location of the machine setup from the World Coordinate System.Since our stock is eight inches in length, we set the X value to -7 in order to keep an inch inside the chuck.

Part 11) Simulate

1. Simulate the part once more and notice our stock is as it should be.
   
   
   
   
2. Exit the Simulation.
   

Part 12) Post the Program and Confirm the Output

After creating all of the necessary features, setting the proper RotationAngle to output, and computing the toolpaths, you post the NC programto confirm the output.

1. In the CAMTree, right-click Milling Job, and click Post.
   
   The program is displayed in the Posting Manager.
   
   

2. Check the program and confirm that the properrotary-axis values are output.

This concludes the example.

Related Topics

IndexingPrograms and Index Systems