Create a Thread Milling Operation

task target This task shows how to insert a Thread Milling operation in the program. For this operation, machining is done in one or more helical passes. 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 Thread Milling .

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

The Thread Milling 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, enter offset values for the Bottom and Contour.
4. If needed, you can invert the tool axis direction by selecting the axis representation in the sensitive icon.
5. Select the Strategy tab page and set the following machining parameters:
  • Machining strategy: Mono-pass or Optimized passes
  • Machining direction: Top to bottom or Bottom to top
  • Approach clearance
  • Machining tolerance
  • Plunge mode 
  • Compensation number depending on those available on the tool
  • Compensation application mode.

Note that the figure displaying the toolpath in this page is different according the Machining strategy and Machining direction settings.

Also note that Breakthrough is not available when the Extension type in the Geometry tab page is set to Blind.
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.

Thread mills or boring bars can be used in this type of operation. If you use a boring bar, machining can be done in Mono-pass mode only. If you use a thread mill in Optimized passes mode, the number of helical toolpaths depends on the effective thread length of the tool and the thread depth of the hole.

Refer to Edit the Tool of an Operation for more information.
6. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

Note that in the toolpath represented in the strategy page shown above, tool motion is at:

  • Motion at machining feedrate from 1 to 2
  • Motion at feedrates defined on macros from 2 to 3 and 3 to 4
  • Retract at retract feedrate from 4 to 5.
7. Select the Macros tab page to specify the operation's transition paths (approach and retract motion, for example). 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.
8. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Thread Milling 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

Note that the helical toolpath is generated with GOTO statements.

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_THREAD_MILLING section of the Manufacturing Infrastructure User's Guide.

end of task