Creating a Spot Drilling Operation

You can create a Spot Drilling operation.

Related Topics
2.5 to 5-Axis Drilling Operations

  1. Activate the Manufacturing Program and click Spot Drilling in the Axial Machining Operations toolbar.

    A Spot Drilling entity is added to the Manufacturing Program. The Spot Drilling dialog box appears directly at the Geometry tab . This tab includes a sensitive icon to help you specify the geometry. Areas of the icon are colored red indicating that this geometry is required.

  2. Still in the Geometry tab.

    See Selecting Geometry

    1. Select red hole depth representation, then select the points to be spot drilled. Double-click to end your selections.

      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.



    2. Click the tool axis to invert the tool axis direction, if required.

  3. Select the Strategy tab to specify the following parameters:

    • Approach clearance (A)
    • Depth mode: By diameter (Dd)

      Note: The diameter value used is the one specified in the Geometry tab.

    • Dwell mode
    • compensation number depending on those available on the tool.

    The other parameters are optional in this case.



  4. Go to the Tool tab to select a tool.

    Drills, Multi-diameter Drills, Spot Drills, Center Drills, and Conical Mills can be used. See Specifying a Tool Element in a Machining Operation.

  5. Select the Feeds and Speeds tab to specify the feedrates and spindle speeds for the operation.

    Note: In our example, the 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.

  6. Select theMacros tab to specify the desired transition paths.

    See Defining Macros on Axial Machining Operations

  7. Click Tool Path Replay to check the validity of the operation.

    See Replaying the Tool Path


    • The tool path is computed.
    • A progress indicator is displayed.
    • You can cancel the tool path computation at any moment before 100% completion.

  8. Click OK to create the operation.

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

    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

    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.

  9. Click Edit Cycle to edit or choose output syntaxes.