Create a Reverse Threading Operation

task target This task shows how to insert a Reverse Threading operation in the program.

To create the operation you must define:

  • the tool that will be used
pre-requisites Open the HoleMakingOperations.CATPart document, then select the desired Machining workbench from the Start menu.  

Make the Manufacturing Program current in the specification tree.
scenario 1.  Select Reverse Threading .

A Reverse Threading entity along with a default tool is added to the program.

The Reverse Threading dialog box appears directly at the Geometry tab page . 
2. Select the red hole depth representation then select a threaded hole feature in the 3D window.
Just double click to end your selection.

The sensitive icon is updated with the following:

  • thread depth and thread diameter
  • hole extension type
  • thread pitch
  • thread direction.

You can modify this data. 
Other values are shown for information only. 
3. If needed, you can invert the tool axis direction by selecting the axis representation in the sensitive icon.
4. Select the Strategy tab page to specify the following machining parameters:
  • approach clearance
  • depth mode: by shoulder
    The depth value used is the one specified in the Geometry tab page.
  • compensation number depending on those available on the tool
  • Compensation application mode.

The other parameters are optional in this case.
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 an Operation.
5. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

Note that in the tool path represented in the strategy page, tool motion is at:

  • Motion at machining feedrate from 1 to 2
  • Spindle off then reverse spindle rotation
  • Retract at machining feedrate from 2 to 3.
6. If you want to specify approach and retract motion for the operation, select the Macros tab page to specify the desired transition paths. The general procedure for this is described in Define Macros of an Axial Machining Operation.
Before accepting the operation, you should check its validity by replaying the tool path.
7. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Reverse Threading operations:

CYCLE/TAP, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE, &MFG_FEED_UNIT, %MFG_CLEAR_TIP

A typical NC data output is as follows:

CYCLE/TAP, 38.500000, 500.000000, MMPM, 2.500000

You can use Edit Cycle to edit or choose output syntaxes. For more information please refer to Editing Cycle Syntaxes in Axial Machining Operations.

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

end of task