Create a Back Boring Operation

This task shows how to insert a Back Boring operation in the program.

To create the operation you must define:

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

Make the Manufacturing Program current in the specification tree.
1. Select Back Boring .

A Back Boring entity along with a default tool is added to the program.

The Back Boring dialog box appears directly at the Geometry tab page . 
2. Select the top plane representation then select the top of the part. 
3. Select the red hole depth representation then specify the hole pattern to be machined by selecting the two counterbored features in the 3D window.

Just double click to end your selections.

The Geometry page is updated with information about the first selected feature.
4. If needed, you can invert the tool axis direction by selecting the axis representation in the sensitive icon.
  5. 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.
6. Select the Strategy tab page to specify the following machining parameters:
  • approach clearances A and A2
  • depth mode: by tip
    The depth value used is the one specified in the Geometry tab page
  • shift: by polar coordinates or linear coordinates
  • retract clearance
  • compensation number depending on those available on the tool
  • Compensation application mode
  • NC output with CYCLE syntax.

See the Reference section for a description of all parameters.
7. 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:

  • Shift motion (if defined) at rapid feedrate from 1 to 2
  • Motion at rapid feedrate from 2 to 3
  • Shift motion (if defined) at rapid feedrate from 3 to 4
  • Motion at machining feedrate from 4 to 5
  • Dwell for specified duration
  • Retract clearance motion at retract feedrate from 5 to 6
  • Shift motion (if defined) at retract feedrate from 6 to 7
  • Retract at retract feedrate from 7 to 8
  • Shift motion (if defined) at retract feedrate from 8 to 9.
8. 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.
  9. Before accepting the operation, you should check its validity by replaying the tool path.

Note that for material removal simulations, Boring Bars are not supported for Photo mode and are not collision checked in Video mode.
10. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Back Boring operations:

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

A typical NC data output is as follows:

CYCLE/BORE, 25.000000, 500.000000, MMPM, 5.000000, ORIENT, 1.000000, 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_BACK_BORING section of the Manufacturing Infrastructure User's Guide.