Create a Chamfering Two Sides Operation

task target This task shows how to insert a Chamfering Two Sides 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 Chamfering Two Sides .

A Chamfering Two Sides entity along with a default tool is added to the program.

The Chamfering Two Sides dialog box appears directly at the Geometry tab page  . 
2. Select the red hole depth representation then select the hole geometry in the 3D window.
Just double click to end your selections.
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 clearances 1 and 2
  • depth mode: by tip
  • dwell in seconds
  • first compensation number depending on those available on the tool for top chamfering
  • second compensation number depending on those available on the tool for bottom chamfering
  • Compensation application mode.

Note that the depth value and chamfer diameter are retrieved from your geometry selections.
A Two Sides Chamfering tool is proposed by default. If the proposed tool is not suitable, just select the Tool tab page to specify the characteristics of 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 as follows:

  • Motion at machining feedrate from 1 to 2
  • Dwell for specified duration
  • Possibly, activation of second tool compensation number (output point change)
  • Motion at approach feedrate from 2 to 3
  • Motion at machining feedrate from 3 to 4
  • Dwell for specified duration
  • Possibly, activation of first tool compensation number (output point change)
  • Retract at retract feedrate from 4 to 5.
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.

Note that for material removal simulations, Two Sides Chamfering tools are not supported for Photo mode and are not collision checked in Video mode.
7. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Chamfering Two Sides operations:

CYCLE/BORE, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE, &MFG_FEED_UNIT, 
            %MFG_CLEAR_TIP, DWELL, %MFG_DWELL_REVOL

A typical NC data output is as follows:

CYCLE/BORE, 25.000000, 500.000000, MMPM, 5.000000, DWELL, 3

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_TWO_SIDES_CHAMFERING section of the Manufacturing Infrastructure User's Guide.

end of task