How to Create a Multiblade Operation (splitters)

Introduction

This tutorial explains how to create a Multiaxis feature which uses the Multiblade toolpath for a part with splitters.

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 Multiblade 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_Hermie_C20U machine.

 

In this example, you create toolpaths that can be used to rough and finish the impeller.

 

Section 1) Roughing

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 Multiblade.

  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.

 

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.

    An example usage is explained later.

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

 

Part 4) Select the Roughing Tool

  1. Click the Tool Crib button.

    The Tool Crib dialog appears.

  2. Select the Tapered tool type on the left of the dialog to show the tapered tools available in the Tool Crib.

  3. Highlight the 0.250 Diameter Tapered and click OK.

    The Tool Crib dialog disappears.

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

 

Part 5) Surface paths

  1. In the Pattern group, set the Strategy to Morph between shroud and hub.

  2. In the Sorting group, update the Method to Zig-zag, start from leading edge.

  3. In the Depth step group, leave the setting to Maximum distance, but update the Distance value to 0.125.

  4. In the Stepover group, change the Maximum distance to 0.125 as well.

    The rest of the values will be left at their default values.

 

Part 6) Part definition

  1. Click the Part definition tab.

  2. Click the ellipses button next to Blades,splitter,fillets to select geometry for the feature.

    The Re/Select Geometry dialog appears.

  3. Select each surface of the three differently colors blades except for the shroud and the trailing edge.



    Selecting the surface in the image below is not necessary.



  4. Click OK.

    The Mill Multiaxis Wizard returns.

  5. Click the ellipses button next to Hub.

    The Re/Select Geometry dialog appears.

  6. Select the hub surface.



  7. Click OK.

    The Mill Multiaxis Wizard returns.

  8. Click the ellipses button next to Shroud.

    The Re/Select Geometry dialog appears.

  9. Select all three shroud surfaces.



  10. Click OK.

    The Mill Multiaxis Wizard returns.

  11. Next to each of the geometry selection buttons is a Stock to leave value. Set all three of these to 0.030.

  12. At the bottom of the Part definition group, set the Number of segments value to 10.

  13. In the Segments group, set Machine to All.

 

Tip: While this tutorial will have you toolpath the entire part, a more common practice is to rough 3 pockets and finish only the blades and splitters the roughing exposes. This allows you to ensure there are no gouges and utilize macros on the machine to complete the rest of the part.

 

Part 7) Tool axis control

  1. Click the Tool axis control tab.

  2. In the Tilting group, set the Side tilt angle to 0.

  3. Click Compute.

 

Part 8) 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 Roughing operation in simulation.

    This will allow you to ensure this operation is free of collisions.

    In this case, we can see there is quite a bit a material left between the blades.



  3. Running a deviation report makes this a little more obvious.



    We will handle this material with the next operation.

    The simulation can take a long time to finish. In this step we will ensure we do not need to simulate this portion of the program again.

  4. In the CutSim tab, select Save Stock.

    The Save As dialog appears allowing you to save the stock.

  5. Update the name to ImpellerRough.STL and save the stock to a location of your choosing.

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

  7. In the CAM Tree, right-click Stock and select Stock Wizard.

  8. The Stock Type is already set to STL n the Stock Specification dialog.

    Set the File Unit to Inch and click Browse.

    The Open dialog appears.

  9. Navigate to the location of the saved stock file and select ImpellerRough.STL and click Open.

    After a moment the Filename appears and the stock is visible in the graphics area.

  10. Click OK.

Section 2) Hub Finishing

Part 1) Copy and Paste the feature

  1. Right-click Feature Multiaxis-Multiblade and click Copy with Geometry.

  2. Right-click the feature again and select Post Yes/No.

  3. Right-click the feature and select Blank/Unblank Toolpath.

  4. Right-click the feature and select Lock/Unlock Operation.

  5. Right-click the feature and and select Rename.

  6. Update the name to Rough and press Enter.

  7. You can also click the small arrow next to the feature to collapse it.

 

Note: By updating the stock with the stl file we saved from the completed simulation, we no longer need to post our Rough operation. We have also hidden the toolpath from view, and locked the operation so it will not be computed if we use the Compute All Toolpath options from the Job, or Machine Setup level of the CAM Tree. This was done after copying the feature because all property features are copied when Copy with Geometry is used. This means we would need to Unlock the operation to compute, and set the operation to post before simulating it.


  1. Right-click Rough and select Paste.

    The Feature Multiaxis-Multiblade operation appears in the CAM Tree under the Rough feature.

 

Part 2) Update the tool

  1. Right-click the new feature and select Edit.

    The Mill Multiaxis Wizard appears.

    Just as in the first feature, we will be leaving the Posting and Multiaxis Post pages as they are.

  2. Click on the tool in the tree to the left to jump to the tool page.

  3. Click Tool Crib.

    The Tool Crib appears.

  4. Click the TAPERED tool group on the left.

  5. Select the 0.1250 Diameter taper tool and click OK.

  6. Click Next.

 

Part 3) Edit the Surface paths

  1. In the Pattern group, set the Machining option to Hub finishing.

  2. In the Sorting group, set the Method to One way, start from leading edge.

  3. In the Stepover group set the Maximum distance to 0.05.

 

Part 4) Part definition

  1. Click the Part definition tab.

    Notice our settings are the same as we set for the Rough feature.

  2. Update the both of the Stock to leave values next to Blades, splitter, fillets and Hub to 0.

  3. Click Compute.


 

Part 5) Simulation

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

  2. Click Step Fwd until the tool engages the material we noticed while simulating the last feature.



    Right away we can see this is too much material to move into.

  3. If we move to the end of the simulation, we will also notice we have a gouge at the ends of our blades.

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

 

Part 6) Updating the feature

  1. In the CAM Tree, right-click the feature and select Blank/Unblank Toolpath.

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

    The Mill Multiaxis Wizard appears.

  3. Click Parameters to jump to the Surface paths tab.

  4. In the First cut group, update Intermediate slices to 3.

  5. Set the Depth step to 0.0625.

  6. Select the First cut feed rate % check box, and set the value to 33.

    This will reduce the feed rate on first pass.

  7. Click Compute.

 

Part 7) Check depth in the simulation

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

  2. Click Step Fwd until the tool engages the material.



    Right away we can see there is much less material being engaged.

  3. Hide the tool, and click in the Measure tab.

  4. Select Distances from the drop-down, and click the scroll wheel of the mouse on the lower edge of the cut we made.



  5. Now use the same scroll wheel click to select the top edge of the cut.



    We can see there is nearly 3/8 of an inch being engaged.

    In this case, we will update the feature one more time to engage a little less material.

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

 

Part 8) Updating the feature

  1. In the CAM Tree, right-click the feature and select Edit.

    The Mill Multiaxis Wizard appears.

  2. Click Parameters to jump to the Surface paths tab.

  3. In the First cut group, update Intermediate slices to 6.

    Leave the Depth step to the current value of 0.0625.

 

Part 9) Check depth in the simulation

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

  2. Click Step Fwd until the tool engages the material.



  3. Hide the tool, and click in the Measure tab.

  4. Select Distances from the drop-down, and click the scroll wheel of the mouse on the lower edge of the cut we made.



  5. Now use the same scroll wheel click to select the top edge of the cut.



    We can see there is just over 1/8 of an inch being engaged, so we will leave it where it is.

  6. Play the rest of the simulation to see how the rest of the hub finishing is applied.

  7. Run another deviation report to ensure this operation is where we need it.



  8. Since the finish looks good, and no gouges are seen, save the stock as HubFinish.stl.

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

 

Part 10) Updating the stock

  1. In the CAM Tree, right-click Stock and select Stock Wizard.

    The Stock Specification dialog opens.

  2. The stock type is already set to STL, so click Browse to search for our new file.

  3. Locate the HubFinish.stl file we just saved and click Open.

  4. When the name appears in the Filename list and you can see the stock in the graphics area, click OK.

    We no longer need to simulate our second feature.

  5. Right-click Feature Multiaxis-Multiblade and select Copy with Geometry.

  6. Right-click the feature and select Post Yes/No.

  7. Right-click the feature and select Lock/Unlock Operation.

  8. Right-click the feature and select Rename, and update the name to Hub Finishing.

Section 3) Blade Finishing

Part 1) Copy the last feature

  1. Right-click Hub Finishing and select Paste.

    Since this feature is a copy of our last, we already have the proper toolpath type selected, the proper tool, the geometry and part definition, as well as our Side tilt angle, set for us already.

 

Part 2) Surface paths

  1. Right-click Feature Multiaxis-Multiblade and select Edit.

  2. Click Parameters in the tree on the left to move to the Surface paths page.

  3. In the Pattern group:

    1. Set Machining to Blade finishing.

    2. Set the Strategy to Offset from hub.

    3. Set the Contour to Full(trim trailing edge).

  4. In the Depth step group set the Distance to 0.03.

 

Part 3) Part definition

  1. Click the Part definition tab.

  2. Click the ellipses button next to Blades,splitter,fillets to select geometry for the feature.

    The Re/Select Geometry dialog appears.

  3. Right-click in the Selected Items list and select Clear Selections.

  4. Select the surfaces of the blade on the left.



  5. Click OK.

    The Mill Multiaxis Wizard returns.

  6. Click Compute.


 

Part 4) Simulation

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

  2. Click Play to view the Finishing operation in simulation.



    Notice toward the bottom of the blade, we begin gouging the blade to the left.

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

  4. In the CAM Tree, right-click the Feature Multiaxis-Multiblade feature, and click Blank/Unblank Toolpath.

 

Part 5) Update the feature

In this toolpath we can also see a lot of extra motion we will try to eliminate.

 

  1. Right-click Feature Multiaxis-Multiblade and select Edit.

  2. Go to the Part definition tab and select the check box for Check surfaces.

  3. Click the ellipses button that appears to open the Re/Select Geometry dialog.

  4. Select the surfaces of the blade to the left of the selected geometry.



  5. Click OK.

  6. Set the Clearance value to 0.01.

  7. Click the Link tab and deselect the check box in the Links between cuts group and the Links between slices group.

  8. Set each Use option in the groups to Blend Spline.

  9. In the Edge tab, set the Edge rolling value to 0.01 as well.

  10. Compute the toolpath.

    Click the operation in the CAM Tree to view the toolpath.

 

Part 6) Simulation

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

  2. Click Play to view the operation in simulation.

  3. Run the deviation report to ensure the desired result has been achieved.



  4. We can see the stock is where we want it to be. Now we repeat the steps used previously: 

    1. Save the stock.

    2. Exit the simulation.

    3. Apply the new stock to the job.

    4. Copy the feature (with geometry).

    5. Set the feature to Post No.

    6. Lock the feature.

    7. Rename the feature to Blade Finishing.

    8. Paste the new feature.

Section 4 Blade Finishing (Splitter)

Part 1) Update the geometry

  1. In the CAM Tree, expand the operation, expand the Geometry folder, right-click Blades, Splitters, Fillets and select Re/Select.

    The Feature Geometry Picking dialog appears.

  2. Right-click in the Selected Items list and select Clear Selections.

  3. Select the surfaces of the splitter.



  4. Click OK.

  5. Right-click the feature and select Compute All Toolpath.



    Notice where the first cut lays on the tip of the blade.



Part 2) Simulation

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

  2. Click Play to view the operation in simulation.

    Notice the bit of extra material on the tip of the splitter.



    As well as the large gouge.



  3. Exit the simulation.

Part 3) Edit the feature

  1. Right-click Feature Multiaxis-Multiblade and select Edit.

  2. In the Pattern group, set the Strategy to Morph between shroud and hub.

  3. Go to the Part definition tab and set the Start offset value next to Shroud to 0.

  4. Click the ellipses button next to Check surfaces to open the Re/Select Geometry dialog.

  5. Select both sides of the each of the large blades on either side of our splitter.



  6. Click OK.

  7. Click the Link tab and set the Links between cuts and Links between slices to Use side arc.

  8. Click the Edges tab and set the Edge rolling value to 0.

  9. Click Compute.

    By comparing the Blade Finishing toolpath to the latest toolpath, you can see how these two methods differ.

     

Part 4) Simulation

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

  2. Click Play to view the operation in simulation.

  3. Run the deviation report to ensure the desired result has been achieved.



  4. We can see the stock is where we want it to be. Now we repeat the steps used previously: 

    1. Save the stock.

    2. Exit the simulation.

    3. Apply the new stock to the job.

    4. Copy the feature (with geometry).

    5. Set the feature to Post No.

    6. Blank the toolpath.

    7. Lock the feature.

    8. Rename the feature to Splitter Finishing.

    9. Paste the new feature.

Section 5) Fillet Finishing (Splitter)

Part 1) Surface paths

  1. Right-click Feature Multiaxis-Multiblade and select Edit.

  2. Click Parameters to jump to the Surface paths page.

  3. In the Pattern group set the Machining option to Fillet finishing.

  4. In the Both sides group:

    1. Set the Number of cuts to 3.

    2. Set the Distance to 0.01.

 

Part 2) Tool axis control

  1. Click the Tool axis control tab.

  2. Set the Min. lead angle to -45.

Part 3) Edges


  1. Click in the Edges tab and set the Edge rolling value to 0.0625.

  2. Click Compute.

 

Part 4) Simulation

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

  2. Click Play to view the operation in simulation.

  3. Run the deviation report to ensure the desired result has been achieved.



    In the image on the top left you can see the previous operation finished much of the fillet as it was finishing the splitter. The image on the top right shows the final finish our last operation achieved.

  4. We can see the stock is where we want it to be. Now we repeat the steps used previously: 

    1. Save the stock.

    2. Exit the simulation.

    3. Apply the new stock to the job.

    4. Copy the Blade Finishing feature (with geometry).

    5. Set the last feature to Post No.

    6. Blank the toolpath for the last feature.

    7. Lock the feature.

    8. Rename the feature to Splitter Fillet.

    9. Paste the new feature.

    10. Unlock the new feature.

 

Important: Since we intend to finish the fillet on the blade, we copy the feature which already has that geometry instead of the previously generated feature.

Section 6) Fillet Finishing (Blade)

Part 1) Surface paths

  1. Right-click the new Blade Finishing and select Edit.

  2. Click Parameters to jump to the Surface paths page.

  3. In the Pattern group set the Machining option to Fillet finishing.

  4. In the Both sides group:

    1. Set the Number of cuts to 3.

    2. Set the Distance to 0.01.

 

Part 2) Tool axis control

  1. Click the Tool axis control tab.

  2. Set the Min. lead angle to -45.

Part 3) Edges


  1. Click in the Edges tab and set the Edge rolling value to 0.0625.

  2. Click Compute.

 

Part 4) Simulation

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

  2. Click Play to view the operation in simulation.

  3. Run the deviation report to ensure the desired result has been achieved.



    In the image on the top left you can see the previous operation finished much of the fillet as it was finishing the splitter. The image on the top right shows the final finish our last operation achieved.

  4. We can see the stock is where we want it to be. Now we repeat the steps used previously: 

    1. Exit the simulation.

    2. Rename the feature to Blade Fillet.

  5. Right-click Milling Job and select Post Yes/No.

    All features and operation are set to not post.

  6. Repeat this step.

    All features and operations are set to post.

  7. Right-click Milling Job and select Blank/Unblank All.

    All toolpath is hidden.

 

 

This concludes the tutorial.

Related Topics

Cuts Along Curve