Manufacturing > Turning > To Create a Profile Turning NC Sequence
  
To Create a Profile Turning NC Sequence
1. Ensure that the active operation references a Lathe or Mill/Turn workcell.
2. Click Turn > Profile Turning. The Profile Turning tab opens.
To create or edit a profile turning step from the Process Manager, perform the following steps:
a. Click Manufacturing > Process Manager. The Manufacturing Process Table dialog box opens.
b. Click or click Insert > Step > Turning step. The Create Turning Step dialog box opens.
c. Specify the Type of step as PROFILE TURNING to insert a new profile turning step.
d. Select a new step or existing step and click Edit Definition to open the Profile Turning tab.
3. Select , , , or for turning on Head 1, Head 2, Head 3, or Head 4.
4. Select a tool from the tool list box. 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.
Alternatively, right-click the graphics window and select Tools.
5. On the Parameters tab, specify the required basic manufacturing parameters. You can also click to define advanced machining parameters or click to copy machining parameters from another step. 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.
6. On the Clearance, Process, and Properties tabs, specify the additional values.
7. On the Tool Motions tab, define the profile turning cut:
 
* The Tool Motions tab is available only after you have defined the mandatory parameters like tool and step parameters.
a. Select Profile Turning from the list on the Tool Motions tab. The Profile Turning Cut dialog box opens.
b. Click the Turn Profile collector and select an existing turn profile.
Alternatively, right-click the graphics window and select Turn Profile Collector.
To create a new turn profile, click Geometry > Turn Profile on the Profile Turning tab. The Turn Profile tab opens. See the Related Links.
c. To select an existing turn profile, click the Turn Profile collector .
Alternatively, right-click the graphics window and select Turn Profile.
d. By default, the cut motion is offset from the turn profile by NOSE_RADIUS (if the OUTPUT_POINT parameter is set to CENTER) as the Offset Cut option is checked. If you want the turn profile to represent the trajectory of the tool control point, rather than the finished geometry, on the Profile Turning Cut dialog box, clear the Offset Cut check box. The cut motion will then coincide with the turn profile.
If you clear the Offset Cut check box, the tool follows the turn profile on the center of the nose radius, violating the reference model geometry.
Alternatively, right-click the graphics window and select Offset Cut.
e. Adjust the cut motion ends under Options.
Alternatively, right-click the graphics window and select Start Collector and End Collector.
f. Specify the corner conditions as Sharp, Fillet, or Chamfer under Corners.
g. Click OK.
8. On the Tool Motions tab, create additional approach motions, exit motions, CL commands, and Goto motions by selecting options from the list.
9. To animate the tool path display, click on the Profile Turning tab. Modify any parameter to adjust the tool path.
10. Click .
 
* You can use the object-action behavior by selecting a predefined Turn profile from the Model Tree and clicking Turn > Profile Turning. After specifying the mandatory step parameters and tool parameters, the tool motion is automatically defined based on the selected turn profile.