How to Create a 4 Axis Rotary Feature


This tutorial explains how to create a 4-Axis Rotary feature.


Example File


The BobCAD part file for this tutorial is available for download at: If you are connected to the Internet, you can click the link provided to download and save the 4 Axis Rotary Example 1.bbcd part file. In the example file provided, the Milling Stock and Machine Setup are already defined for the part. The program is simulated using the BC 4x Mill, which is a 4 axis machine with an A-axis rotary.

Part 1) Add the Feature

Step 1.    To insert a 4 Axis Rotary feature, in the Data-CAM Tree Manager, click the CAMTabIconBBCD.png CAM Tree tab.


Step 2.    Next to MillingStockIconWhite.png Milling Stock, click ExpanderPlus.png to expand the tree.


Step 3.    Right-click MachineSetupIcon.png Machine Setup, and click Mill 4 Axis Rotary. The 4 Axis Wizard dialog box is displayed.

Part 2) Select Geometry

Step 1.    In the Geometry Selection dialog box, click Select Geometry, and select the part geometry for the feature. For this example, select the entire part by clicking and dragging a window around the part. The geometry changes to the selection color to show that it is selected.


Img  Img



Step 2.    To confirm the geometry selection, click OKCheckmarkIconWhite.png (OK). The 4 Axis Wizard dialog box is displayed.


Step 3.    Click Next>> to finish the Geometry Selection dialog box and begin editing the feature parameters.


Step 4.    In the Feature 4 Axis Rotary dialog box, notice that the Clearance Plane has been automatically set using the value defined earlier in the Machine Setup dialog box. (The Machine Setup was previously defined in the provided example file.) The Rapid Plane value is also set to this value by default. In the Rapid Plane box, type 0.500.


Step 5.    In the Feed Plane box, type 0.250.


Step 6.    Notice that the Top of Part is automatically set based on the selected geometry and machining origin.


Step 7.    Click Next>> to open the Posting dialog box. The Work Offset value is also automatically set to the value defined in the Machine Setup dialog box. Click Next>> to open the Rough dialog box.

Part 3) Define the Tool Parameters

Step 1.    In the Tool Data group, clear the CheckBoxCleared.png System Tool check box.


Step 2.    Set the Diameter to 0.500, the Flute Length to 3.000, the Corner Radius to 0.250, and the Overall Length to 5.000.


Step 3.    To assign a tool holder to the tool for the feature, click Assign Tool Holder.


Step 4.    In the Milling Tool Holder Library, in the CAT 40 Holder list, click 0.5 inch I.D. Arbor CAT 40. The row of the selected arbor changes color to show that it is selected.


Step 5.    To confirm the selection and assign the selected holder, click OK.


Step 6.    To finish the tool definition and go to the Patterns dialog box, click Next>>.

Part 4) The Pattern Dialog Box

Step 1.    In the Cut Pattern group, to define one-way cutting, select Zig.


Step 2.    Next to Style, select Around.


IMPORTANT:     To create proper toolpaths with the Rotary feature, you must define the Direction and Base Point for the rotational axis of the part. The values used to set the Base Point are based on where the Machine Setup (machining origin) is located in reference to the center of rotation for the part. If you place the machining origin in-line with the rotary axis, then the Base Point values are set to zero. Placing the machining origin on the rotational axis of the part means there is no difference to report between the machining origin and the rotary axis. In this scenario, although the Base Point values are zero, the Direction of the rotary axis must still be properly defined.


Step 3.    The Rotary Axis must be defined for the part. To set the direction of the rotary axis, in the Rotary Axis group, select X Axis. Because the machining origin was moved away from the center of rotation, this difference must be defined using the Base Point parameter. The following image shows the distance that is used to set the base point. This is the distance from (1) the Machine Setup (machining origin) to (2) the center of rotation. (You can click the MachineSetupIcon.png Machine Setup item in the CAMTabIconBBCD.png CAM Tree to view the Machine Setup, or machining origin.)





Step 4.    The only difference to report for this example is along the Z-axis. The radius of the part (and stock) is 3.2679 inches. In the Base Point group, in the Z-box, type -3.2679.


Step 5.    In the Cut Direction group, select Clockwise.


Step 6.    To finish the Patterns dialog box, click Next>>.

Part 5) The Parameters Dialog Box

Step 1.    In the Finish group, in the Stepover box, type 0.100.


Step 2.    To leave material for finishing, in the Allowance XYZ box, type 0.050.


Step 3.    To calculate the toolpath, click Compute.





Step 4.    Notice that a single toolpath pass is created for the entire length of the part. The next step is to edit the feature and use the Along Rotary Axis options to limit the area of the part that is cut.

Part 6) Edit the Feature and Limit the Toolpath

Step 1.    When you computed the toolpath, the FeatureIconWhite.png Feature 4Ax-Rotary was added to the CAMTabIconBBCD.png CAM Tree. To edit the feature, in the CAM Tree, right-click 4AxisRotaryFeatureIcon.png 4Ax-Rotary, and click Edit.


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


Step 3.    In the Along Rotary Axis group, select the CheckBoxSelected.png End check box, and type 4.00. The toolpath now ends 4 inches from the Machine Setup instead of cutting the entire part. (You can also limit the toolpath by changing the Start parameter to define where the toolpath starts in relation to the Machine Setup, along the defined Rotary Axis Direction.)

TIP:   You can use the Along Rotary Axis parameters Start and End, to define where the toolpath starts and ends. (By default, the Rotary feature creates the toolpath by cutting in the positive direction along the selected rotary axis. For example, with a A-axis rotary (rotation around the X-axis) the toolpath is from left to right.)





Step 4.    To add the changes and view the results, click Compute.



Part 7) Create Multiple Passes

Step 1.    The next step is to add multiple passes to the feature. Edit the feature, and on the left side of the dialog box, click Parameters.


Step 2.    In the Multiple Passes group, select the CheckBoxSelected.png Multiple Passes check box to enable the Roughing Passes and Finishing Passes groups.


Step 3.    In the Roughing Passes group, in the Numbers box, type 2.00, and in the Spacing box, type 0.250.


Step 4.    Next to Sort By, select Passes. This causes the feature to cut each pass before moving on to the next pass. In other words, this cuts the entire part to one depth before moving on to the next depth.


Step 5.    To view the results, click Compute. The toolpath now contains two passes instead of the single pass created earlier. Notice that the multiple passes start from the surface and not the top of the part.


Img Img

Part 8) Change the Cut Interval

Before simulating the program, there is one last change to make. You can see in the previous step that the tool is plunging, at rapid rate, into one of the deepest areas of the part geometry. The next steps cause the tool to plunge into a much more shallow area of the part.


Step 1.    Edit the feature, and click Patterns.


Step 2.    In the Angular Start/End group, select the Cut Interval option.


Step 3.    In the Angle Start box, type -135.


Step 4.    In the Angle End box, type 225.


Step 5.    To add the changes and view the result, click Compute. The result is shown next.


Img Img

Part 9) Simulate the Program

Step 1.    To view the part being cut, in the Modules menu, click MillSimulationIconBBCD.png Mill Simulation. To learn more about using simulation, view the Getting Started with Simulation help topic.





Step 2.    For this example, it is important to understand the Work Offset parameter that was previously defined in the Machine Setup dialog box. To open the Machine Setup dialog box, in the CAMTabIconBBCD.png CAM Tree, right-click MachineSetupIcon.png Machine Setup, and click Edit.


Step 3.    In the Machine Setup dialog box, click Work Offset. Notice the values in the Work Offset dialog box. These values represent the distance from the machine zero to the part zero (that is defined by the Machine Setup). For this example, this is from the center of the face of the rotary table to the machining origin that is on the top of the cylindrical stock.


Step 4.    Again, when the machining origin is not the same as the machine zero, you must define the difference between these two coordinate systems using the Work Offset dialog box. This is necessary to create proper machine simulation.



This concludes the tutorial. To learn about any parameters not explained in this tutorial, view the 4 Axis Rotary feature help topic.