To Create HSM Rough Sequences
1. Ensure that the active operation references a Mill or Mill/Turn work center.
 |
The  HSM Rough command with 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 Rough in the High Speed Milling group. The HSM Rough tab opens.
HSM Rough in the High Speed Milling group. The HSM 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.
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.
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.
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:
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 for the 3 axis or 3+2 axis machining:
◦ Machining Reference—For 3 axis machining, select a mill window or mill volume from the graphics area or Model Tree. For 3+2 axis machining, select a mill volume from the graphics area or Model Tree.
| | • Mill window is not applicable for 3+2 axis machining. You cannot select a mill window for 3+2 axis machining. • If you remove a machining reference, it is removed for both 3 axis and 3+2 axis machining. |
All the surfaces within the specified mill window or mill volume are machined. Alternatively, right-click the graphics window and select Machining Reference. Then, select the following:
▪ Mill window or mill volume for 3 axis machining.
▪ Mill volume for 3+2 axis machining.
| | You can select a mill volume for 3+2 axis machining in the Machining Reference collector. However, selection of a machining reference is not mandatory for 3+2 axis machining to generate a toolpath. |
To create a new mill volume, click 
Geometry > 
Mill Volume on the HSM Rough tab. The Mill Volume tab opens.
Geometry > Mill Volume on the HSM Rough tab. The Mill Volume tab opens.To create a new mill window on the fly in 3 axis machining, click Geometry > Mill Window on the HSM Rough tab. The Mill Window tab opens.
Geometry > Mill Window on the HSM Rough tab. The Mill Window tab opens.| | • Tool Side option is considered if ALLOW_ENTRY_OUTSIDE parameter is set to NO. • The References tab is available for 3 axis and 3+2 axis machining. • If you switch from 3 Axis to 3+2 Axis machining on the Axis Control tab and a mill window is selected for 3 axis machining, the selection is ignored for 3+2 axis machining. |
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.
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.
to copy cutting tool adapter from another step.10. On the Tool Motions tab, define the following:
◦ Goto Point—Create a Goto Point tool motion. For more information, see To Create a Goto Point Tool Motion.
◦ CL Command—Insert a CL command along the toolpath. For more information, see To Insert a CL Command for Tool Motions.
| | The Tool Motions tab appears only when you define machining references. |
11. On the Axis Control tab, set the following options:
◦ Type—Select 3 Axis for 3 axis machining or select 3+2 Axis for positional machining. In 3+2 or positional machining, you create a 3 axis milling toolpath with different machining orientations that are automatically decided to achieve maximum material removal.
◦ Search Angle Increment—Specify the angle increment in degrees. While searching for the optimal machining direction to avoid collisions and gouges, the tool tilts in increments of the specified value. The search angle must be from 1 through 90.
◦ Min Stock to Detect Area—Specify the stock thickness. The unmachined stock is detected and machined in iterations. If the stock thickness of the unmachined area is lesser than the specified value, the area is not detected and the toolpath is not generated.
This value must be greater than the sum of ROUGH_STOCK_ALLOW or BOTTOM_STOCK_ALLOW and TOLERANCE parameters.
◦ Max Tilt Angle—Specify the maximum angle in which the tool can be tilted from the Z axis. The angle must be from 5 through 90.
| | The Axis Control tab is available for the 5 axis Mill or 5 axis Mill-Turn Work Center. |
12. 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.
to automatically calculate the machining time for the step. The Calculated Time box shows the time.◦ Actual Time—Specify the machining time.
13. 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.
—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
—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.
—Save current step comments in a text file.▪ 
—Accept the current step comments.
—Accept the current step comments.14. Click 
button to open a separate CL Data window.
button to open a separate CL Data window.15. Click 
to get a dynamic preview of the tool path in the graphics window.
to get a dynamic preview of the tool path in the graphics window.16. After you define the mandatory step elements, select a command for toolpath validation:
◦ To play the toolpath, click the arrow next to 
and select .
and select .◦ To recompute the toolpath, click the arrow next to and select 
.
and select .◦ To perform gouge checking against surfaces of the reference part, click the arrow next to and select 
.
and select .◦ To view the simulation of material removal as the tool is cutting the workpiece, click the arrow next to and select 
. The Material Removal tab with integrated simulation environment opens.
and select . The Material Removal tab with integrated simulation environment opens.17. Select one of the following options to complete the sequence:
◦ Click 
to save the changes.
to save the changes.◦ Click 
to pause the process and use one of the asynchronous tools. Click 
to resume.
to pause the process and use one of the asynchronous tools. Click to resume.◦ Click 
to cancel the changes.
to cancel the changes.