Create a Thread Turning Operation

task target This task shows how to insert a Thread 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 Thread Turning icon .

A Thread Turning entity along with a default tool is added to the program.

The Thread Turning dialog box appears directly at the Geometry tab page . 
This tab 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.
2. Click the red part in the icon then select the desired part profile in the 3D window.
3. Specify the desired length of threading.
4. Select the Strategy tab page to specify the main machining parameters that are organized in three tabs: Thread, Strategy and Options. 

Set the following values in the Thread tab:

  • Profile: Other
  • Orientation: External
  • Location: Front
  • Thread unit: Pitch
  • Number of threads: 1
  • Thread depth: 10mm
  • Thread pitch: 10mm.

Other optional parameters can be set in the Strategy and Options tabs.

5. If you want to generate CYCLE statements, you must select the Output CYCLE syntax checkbox in the Options tab and set the Syntax Used option to Yes in the NC Output generation dialog box. Otherwise, GOTO statements will be generated. 

You can display and edit CYCLE syntaxes by clicking the Edit Cycle command.
  6. 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.
7. Select the Feeds and Speeds tab page to specify the machining spindle speed for threading.

Feedrates in units per minute are available for air cutting such as macro motions and path transitions.
Note that RAPID feedrate can be replaced by Air Cutting feedrate in tool trajectories (except in macros) by selecting the corresponding checkbox.
8. Select the Macros tab page to specify the operation's transition paths (approach and retract motion, for example). 

See Define Macros on a Lathe Operation for an example. 
  9. Before accepting the operation, you should check its validity by replaying the tool path.
10. Click OK to create the operation.

Example of output

If your PP table is customized with the following statement for Thread Turning operations:

CYCLE/THREAD,%MFG_THREAD_PITCH

A typical NC data output is as follows:

CYCLE/THREAD, 10.000000

The parameters available for PP word syntaxes for this type of operation are described in the NC_LATHE_THREADING section of the Manufacturing Infrastructure User's Guide.

end of task