Create a Profile Finish Turning Operation

task target This task shows how to insert a Profile Finish Turning operation in the program. To create the operation you must define:
pre-requisites Open the Lathe01.CATPart document, then select Machining > Lathe Machining from the Start menu. Make the Manufacturing Program current in the specification tree.  
scenario 1. Select the Profile Finish Turning icon .

The Profile Finish Turning dialog box appears directly at the Geometry tab page . 
This page includes a sensitive icon to help you specify the geometry to be machined.

The part in the icon is colored red indicating that this geometry is required for defining the operation. 
2. Click the red part in the icon, then select the desired part profile in the 3D window.
3. In addition to the global offsets that you can assign to the selected profile, you can also add local values.

Right-click the geometry to be assigned the local value, and select the Add Local Information contextual command. A dialog box appears allowing you to assign the desired local values.

Other contextual commands are available for analyzing and resetting local information. Please refer to Local Information for more details. 
The part of the icon is now colored green indicating that this geometry is now defined.
4. Select the Strategy tab page to specify the general machining strategy parameters:
  • Orientation: External
  • Location: Center
  • Select the Recess machining checkbox
  • Machining direction is set automatically To spindle.

Note that you can locally invert machining directions using Local Information facilities.
Other optional parameters can be set in the Machining, Corner Processing, and Local Invert tabs.
A tool is proposed by default when you want to create a machining operation. If the proposed tool is not suitable, just select the Tool tab page to specify the tool you want to use. This is described in Edit the Tool of a Lathe Operation.

Note that if a Limit mode (Start Limit or End Limit) is selected, then an insert with more than one tool radius (such as a Groove insert) is not compatible.

5. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation. See Feeds and Speeds for Profile Finishing for more information.
In addition to the global feedrates that you can assign for the operation, you can also add local feedrates to portions of the profile. 

Right-click the geometry to be assigned the local value, and select the Add Local Information contextual command. A dialog box appears allowing you to assign the desired local values.

Other contextual commands are available for analyzing and resetting local information.  Please refer to Local Information for more details. 
You can add approach and retract motions to the operation in the Macros tab page . See Define Macros on a Lathe Operation for an example. 
6. Check the validity of the operation by replaying the tool path.
7. Click OK to create the operation.

end of task