Turn Mill Example 2

Introduction

This tutorial explains how to create a Turn Mill operation and adjust some of the most commonly used settings.

Example File

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 Turn Mill Example 2.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 Tool Crib is already equipped with the necessary tools and the stock and Machine Setup are already defined. The part is simulated using the BC_Porting_4x_HeadTable_Rotary_Only machine.

 

Part 1) Add the Feature

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

2. Right-click Machine Setup and click Mill Multiaxis.
   
   

3. In the Multiaxis Wizard, click Turn Milling.
   
   

4. Click Next>> to go to the Posting dialog box.

Part 2) Define the Posting Parameters

1. The Work Offset # is automatically set to the value defined in the Machine Setup dialog box.
   
   You can change the value here to update the Work Offset # for the feature.
   
   

2. Click Next>> to go to the Multiaxis Posting dialog box.

Part 3) Define the Multiaxis Posting Parameters

1. Notice, at the top of the dialog box, that the Use Machine Settings check box is selected.
   
   This means that the Multiaxis Posting parameters for the feature use the same parameters as the machine that is selected in Current Settings.
   
   You can clear the Use Machine Settings check box to define the Multiaxis Posting parameters of the feature separately from the current machine settings.
   
   For this example, no changes are needed (more information is provided later).
   
   

2. Click Next>> to go to the Tool page.

Part 4) Define the Tool Parameters

1. In the Tool page, click Tool Crib.
   
   The Tool Crib dialog appears.
   
   

2. Select the Rough+2 tool and click OK.
   
   The Tool Crib disappears and the Rough+2 tool is now assigned.
   
   

3. Click Next>> to go to the Parameters.

Part 5) Surface paths

1. In the Sorting group, set the Axial moves to Bi-directional / Positive.
   
   This sets tool to cut back and forth along the axis, and forces it to begin in a positive direction.
   
   
   
   

2. In the Depths steps group set the Distance to 0.125.
   
   

3. In the Stepover group set the Max. stepover to 0.250.

Part 5) Part definition

Step 1) Select the Part surface

 

1. Click on the Part definition tab to jump to define the geometry.
   
   

2. Next to Part, click the drop down on Turn profile and set it to Part surface.
   
   This will allow us to select the solid as geometry rather than using a wireframe profile.
   
   

3. Click the ellipses button next to Part surface.
   
   The Mill Multiaxis wizard disappears and the Re/Select Geometry dialog appears.
   
   

4. Select the check box for Select whole bodies.
   
   

5. Select the model.
   
   
   
   

6. Click OK.
   
   The Mill Multiaxis Wizard returns.

 

Step 2) Set the Stock to leave and the Axis of rotation

1. Set the Stock to leave value to 0.05.
   
   

2. Click the Axis of rotation button.
   
   The Rotation axis dialog appears.
   
   

3. By default the By base point and direction option is selected.
   
   Set the Direction to X, and click OK.
   
   The dialog disappears.

 

Step 3) Limit the Machining area

 

1. In the Part definition group click the Machining area button.
   
   The Machining area dialog appears.
   
   

2. In the User limits group select the check box for Axial.
   
   

3. Click the ellipses button.
   
   The Axial limit dialog appears.
   
   

4. Click the ellipses button to the right of the dialog.
   
   The dialogs disappear and the Re/Select Geometry dialog opens.
   
   

5. Select the Pick two points option.
   
   

6. Click in the End Point list to give it focus, and select the back edge of the part.
   
   
   
   

7. Click OK in the Axis limits dialog.
   
   

8. Click OK in the Machining area dialog.
   
   

9. Click Compute.
   
   
   
   Notice we are not machining all the way to the back of the stock.

Part 7) Simulation

For more help using simulation, view Getting Started with Simulation.

 

1. To view the program, in the Quick access menu of the CAM Tree, click Simulation.
   
   

2. Click Play to view the current operation.
   
   Notice at the start of the pass the tool is to the -Y side of the rotation axis.
   
   
   
   At the start of the next pass the tool is to the +Y side of the rotation axis and the chuck is spinning the other way.
   
   
   
   This is done to continue our climb engagement while allowing Bi-directional axial moves.
   
   

3. With Popup Notifications set to Collision & Gouge the simulation will stop to warn of a crash.
   
   
   
   Exit out of the Gouge/Collision dialog.
   
   

4. Set the Stock to Transparent and the Workpiece to Show.
   
   
   
   The arbor is coming into contact with the stock before the final depth is reached.
   
   We will correct this by limiting the Radial User limits of the Machining area.
   

    

5. To close simulation, in the BobCAM menu, click Exit Simulation.
   

Part 8) Edit the Machining area

1. Right click the feature in the CAM Tree and select Edit.
   
   

2. Click Parameters in the tree on the left of the wizard.
   
   

3. Click the Part definition tab.
   
   

4. In the Part definition group click the Machining area button.
   
   The Machining area dialog appears.
   
   

5. In the User limits group select the check box for Radial.
   
   

6. Click the ellipses button.
   
   The Axial limit dialog appears.
   
   

7. Click the ellipses button to the right of the dialog.
   
   The dialogs disappear and the Re/Select Geometry dialog opens.
   
   

8. Select the Pick two points option.
   
   

9. Click in the End Point list to give it focus, and select the edge seen in the image below.
   
   
   
   

10. Click OK.
    
    The dialog disappears.
    
    

11. Click OK in the Axial limits dialog.
    
    Notice the values for the Start and End.
    
    

12. Click OK in the Machining area dialog.
    
    

13. Click Compute.
    
    
    
    This is clearly not the desired result.
    

Part 9) Understanding the Radial limits

Important: The radial start begins from the center of rotation. With a Start of zero, and the end at our specified distance we are only doing the last few depths of the part.

 

1. Right-click the feature in the CAM Tree and select Copy with Geometry.
   
   

2. Right-click the feature again and select Paste.
   
   The copy is added to the CAM Tree.
   
   

3. Right-click the original feature and select Edit.
   
   

4. Right-click Parameters in the tree on the left.
   
   

5. Click the Part definition tab.
   
   

6. In the Part definition group click the Machining area button.
   
   The Machining area dialog appears.
   
   

7. Click the ellipses button next to Radial.
   
   The Axial limit dialog appears.
   
   

8. Click the ellipses button to the right of the dialog.
   
   The dialogs disappear and the Re/Select Geometry dialog opens.
   
   

9. Select the Pick two points option.
   
   

10. By default the Start Point list has focus. Click the top edge seen in the image below.
    
    
    
    

11. Click in the End Point list to give it focus, and select the edge seen in the image below.
    
    
    
    

12. Click OK.
    
    The dialog disappears.
    
    

13. Click OK in the Axial limits dialog.
    
    Notice the values for the Start and End.
    

 

Tip: The points selected for the Start and End could be reversed and the values will remain the same for each. The larger of the two values is automatically assigned to the End value.

 

14. Click OK in the Machining area dialog.
    
    

15. Click Compute.
    
    

Part 10) Simulation

For more help using simulation, view Getting Started with Simulation.

 

1. To view the program, in the Quick access menu of the CAM Tree, click Simulation.
   
   

2. Click Play to view the current operation.
   
   

3. Set the Stock to Transparent and the Workpiece to Show.
   
   
   
   Notice we no longer have a collision, but we now are not machining to the part in the front and back.
   
   We will complete this last portion with the feature we copied into the CAM Tree.
   

    

4. To close simulation, in the BobCAM menu, click Exit Simulation.
   

Part 11) Edit the second feature

1. Right-click the first feature and select Blank/Unblank.
   
   

2. Right-click the second feature and select Edit.
   
   

3. Click Rough in the tree on the left.
   
   

4. Click Tool Crib.
   
   The Tool Crib dialog appears.
   
   

5. Select Tool Number 2 and click OK.
   
   

6. Click Next>>.
   
   

7. In the Stepover group, set the Max. stepover to 0.16.
   
   

8. Click Compute.
   
   
   

 

Part 10) Simulation

For more help using simulation, view Getting Started with Simulation.

 

1. To view the program, in the Quick access menu of the CAM Tree, click Simulation.
   
   

2. Click Next Op to skip our first operation.
   
   

3. Set the Stock to Transparent and the Workpiece to Show.
   
   
   
   

4. Click Play to view the current operation.
   
   
   
   We can see the part is now completely roughed.
   

5. To close simulation, in the BobCAM menu, click Exit Simulation.
   

 

This concludes the example.

Related Topics

Cuts Along Curve