Manufacturing > Manufacturing > High Speed Milling > To Create Auto Deburring Sequences
To Create Auto Deburring Sequences
1. Ensure that the active operation references a Mill or Mill/Turn workcell.
* 
The Mill/Turn work center is available when you have both the Complete Machining and ModuleWorks-based Mold Machining licenses.
2. Click Mill > Auto Deburring in the High Speed Milling group. The Auto Deburring tab opens.
3. Depending on the type of workcell the operation references, select one of the following:
◦ 3 axis machining
◦ 5 axis machining
4. Click Tool Manager or select Edit Tools from the tool list box to open the Tools Setup dialog box and add a new cutting tool or change tool parameters. The tool list only includes tools that are valid for the step.
* 
To show tools for the current step and the active head on the machine tool, set the INCLUDE_ALL_TOOLS_IN_LIST option to YES.
Alternatively, right-click in the graphics window and select Tools.
5. To preview the cutting tool and its orientation in the graphics window, click adjacent to the right of the tool list box. The button becomes available once a tool is selected.
Alternatively, right-click the graphics window and select the Tool Preview option on the shortcut menu. After you select a tool, the Tool Preview option is available on the shortcut menu of the graphics window.
To exit the tool preview, right-click the graphics window and select Cancel tool preview from the shortcut menu or click the button again.
6. To change the coordinate system that defines the orientation of the step, click the collector adjacent to and select a coordinate system. If the operation coordinate system differs from the step coordinate system, right-click the collector for the following options:
◦ Default—Replaces the selected coordinate system with the default reference. The default is the orientation that is copied from the previous step or from the operation.
◦ Information—Displays the information of the selected coordinate system.
* 
After you specify a coordinate system for an NC sequence, it remains in effect until you change it.
Alternatively, right-click the graphics window and select Orientation from the shortcut menu.
7. Select the following options on the References tab:
◦ Reference part—Click in the box and select a reference part in the graphics window. Alternatively, right-click in the graphics window and select Reference Part.
◦ Include all edges—By default all edges in a reference part are machined. Clear the selection by clicking the option.
▪ Exclude edges—Select the edges that you do not want to machine.
▪ Include edges—When you clear the Include all edges option, you can select the edges that you want to machine.
8. On the Parameters tab, specify the required manufacturing parameters.
You can also click to copy parameters from an earlier step or click to edit parameters specific to High Speed Finish. By default, the required parameters for the selected tool are defined by relations that you can modify from the Relations dialog box.
Alternatively, right-click the graphics window and select Parameters from the shortcut menu.
9. On the Clearance tab, optionally specify the following:
◦ Retract—Specify the Type, Reference, and Value for the retract definition. For 5 axis sequences, the retract type is set to Automatic by default.
◦ Start and End Points—Specify the Start point and End Point for the step tool path.
Alternatively, right-click the graphics window and select the Start Point and End Point of the cutting tool from the shortcut menu.
10. On the Options tab, open a part or assembly to use as a cutting tool adapter. Alternatively, click to copy cutting tool adapter from another step.
11. On the Axis Control tab, set the following options:
◦ Tilt Angle—Specify the angle in which the tool can be tilted from the Z axis. The angle must be from –180 through 180.
◦ Max Tilt Angle—Specify the maximum angle in which the tool can be tilted from the Z axis. The angle must be from 0 through 180.
* 
The Axis Control tab is available for the 5 Axis Mill or Mill-Turn Work Center.
12. Use options on the Check Surfaces tab to define the parts and surfaces that can be used as a limit on the tool motions during machining.
Alternatively, right-click the graphics window and select Check Surfaces.
13. On the Process tab, optionally use any of the following options for the machining step:
◦ Calculated Time—Click to automatically calculate the machining time for the step. The Calculated Time box shows the time.
◦ Actual Time—Specify the machining time.
14. On the Properties tab, optionally specify the name or comments for the step.
◦ Name—Displays the name of the step. You can type another name.
◦ Comments—Type the comments associated with the step in the text box or use the following options:
▪ —Read in an existing text file containing step comments and replace any current step comments.
▪ —Insert the contents of an existing text file of step comments at the cursor location. Preserve any current step comments
▪ —Save current step comments in a text file.
▪ —Accept the current step comments.
15. Click button to open a separate CL Data window.
16. Click to get a dynamic preview of the tool path in the graphics window.
17. After you define the mandatory step elements, the following buttons become available in a drop down list:
◦ To play the tool path, click .
◦ To perform gouge checking against surfaces of the reference part, click .
◦ To view the simulation of material removal as the tool is cutting the workpiece, click . The Material Removal tab with integrated simulation environment opens.
18. Select one of the following options to complete the sequence:
◦ Click to save the changes.
◦ Click to pause the process and use one of the asynchronous tools. Click to resume.
◦ Click to cancel the changes.