Create a Spot Drilling Operation

task target This task shows how to insert a Spot Drilling 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 Spot Drilling .

A Spot Drilling entity along with a default tool is added to the program.

The Spot Drilling dialog box appears directly at the Geometry tab page . This tab page includes an icon representing a simple hole. There are several hot spots in the icon.
2. Select red hole depth representation, then select the points to be spot drilled. 
You can do this by selecting the circular edges of holes.
In this case, the circle centers are taken as the points to be spot drilled.
Just double click to end your selections.
3. If needed, click on the tool axis symbol to invert the tool axis direction.
4. Select the Strategy tab page to specify the following machining parameters:
  • approach clearance
  • depth mode: by diameter
    The diameter value used is the one specified in the geometry tab page.
  • dwell
  • compensation number depending on those available on the tool
  • Compensation application mode.

The other parameters are optional in this case.
  5. A tool is proposed by default when you want to create a machining operation. 

Drills, Multi-diameter Drills, Spot Drills, and Center Drills can be used.
Conical Mills can also be used.

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 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 the specified duration
  • Retract at retract feedrate from 2 to 3.
7. 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.
  8. Before accepting the operation, you should check its validity by replaying the tool path.
9. Click OK to create the operation.
Example of output

If your PP table is customized with the following statement for Spot Drilling operations:

CYCLE/SPDRL, %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/SPDRL, 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_SPOT_DRILLING section of the Manufacturing Infrastructure User's Guide.

end of task