To Create a Profile Milling NC Sequence
1. Ensure that the active operation references a Mill or Mill/Turn workcell.
2. Click
Mill >
Profile Milling.
The Profile Milling tab opens.
3. Depending on the type of workcell the operation references, select one of the following:
◦ 
—3–axis machining.
◦ 
— 4–axis machining.
◦ 
—5–axis machining.
4. Select
,
,
, or
for milling on Head 1, Head 2, Head 3, or Head 4.
|  The Head Selector options are available only if the operation references a Mill-Turn or Lathe, and if both heads are activated in the work center. |
5. 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.
6. 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.
7. 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.
| 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.
8. On the References tab, select Surface or Previous Step from the Type list.
Alternatively, right-click the graphics window and select Machining References from the shortcut menu.
| Selecting the surfaces or previous step before entering the Profile Milling tool adds them to the machining references collector automatically. |
◦ Scallop Surfaces—Select surfaces to be excluded from scallop computation if you have specified a value for the SCALLOP_HGT parameter.
9. 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 profile milling. By default, the required parameters 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.
10. On the Clearance tab, specify additional parameters if required by selecting appropriate options.
11. 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.
12. On the 4-axis Plane tab, select a plane to which the tool axis is parallel, if you are creating 4-axis milling steps.
13. On the Options tab, select any of the following options if required:
◦ Cutting Tool Adapter—Select a part or assembly to use as a cutting tool adapter.
◦ Approach Axis—Select an axis to be used by the tool as an approach to the surface being machined.
◦ First Slice Only—Select this check box to apply the approach motion to the first slice.
◦ Exit Axis—Select an axis to be used by the tool as an exit to the surface being machined.
◦ Last Slice Only—Select this check box to apply the exit motion to the last slice.
14. On the Tool Motions tab, select the options to create, modify, and delete tool motions and CL commands for defining cut motions. For details on all the tool motions, see the topics under Related Links.
Alternatively, right-click the graphics window and select Tool Motion Options.
| With the Return to Step Options on the shortcut menu in the graphics window you can switch from editing tool motions and editing step references. This option is available only when all references for tool path computation are successfully defined. |
15. Click
to get a dynamic preview of the tool path in the graphics window.
16. 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.
◦ Prerequisites—Click
. The
Select Step dialog box opens. Select an existing step that is a prerequisite for the new trajectory milling step. Click
OK.
| The Prerequisites option is available on the Process tab while creating or editing a step from the Process Manager. |
17. 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.
18. After you define the mandatory step elements, the following buttons become available:
◦ 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.
19. 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.