Manufacturing > Manufacturing > High Speed Milling > To Create HSM 5 Axis Rough Sequences
To Create HSM 5 Axis Rough Sequences
1. Ensure that the active operation references a 5 axis Mill or Mill/Turn work center.
* 
The Mill/Turn work center is available when you have both the Complete Machining and ModuleWorks-based Mold Machining licenses.
2. Click Mill and then click HSM 5 Axis Rough in the High Speed Milling group. The HSM Multi Axis Rough tab opens.
3. 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.
4. To preview the cutting tool and its orientation in the graphics window, click 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 button again.
5. 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 commands:
◦ 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.
If your work center setup has two spindles, choose Main Spindle or Sub Spindle from the list and select a coordinate system each for the main and sub spindle.
* 
The sub spindle is available when you have both the Complete Machining and ModuleWorks-based Mold Machining licenses. 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.
6. Select the following option on the References tab:
◦ Slice Generation Strategy—Select an offsetting strategy for the slices in the toolpath.
▪ Offset from Floor—Create a toolpath where slices offset from the selected floor surface.
▪ Offset from Ceiling—Create a toolpath where slices offset from the selected ceiling surface.
▪ Morph—Create a toolpath that morphs from floor surface to ceiling surface or vice-a-versa while offsetting.
◦ Floor Surface—Select individual surfaces or click Details and select surface sets from the graphics window. Right-click and click Remove to remove the surfaces.
◦ Ceiling Surface—Select individual surfaces or click Details and select surface sets from the graphics window. Right-click and click Remove to remove the surfaces.
◦ Containment Loops—Select individual closed loops or click Details and select chains of loops. These loops are perpendicularly projected on the floor surface and areas inside the loops are machined.
7. 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 Rough step. 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.
8. On the Clearance tab, optionally specify the following:
◦ Retract—Specify the Reference and Value for the retract definition
◦ Start and End Points—Specify the Start point and End Point for the step tool path.
Alternatively, right-click the graphics window and select Retract. You can also select the Start Point and End Point of the cutting tool from the shortcut menu.
9. 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.
10. 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.
11. 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.
12. Click button to open a separate CL Data window.
13. Click to get a dynamic preview of the tool path in the graphics window.
14. 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.
15. 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.
High Speed Milling Parameters