Creating a Tapping Operation

You can create a Tapping operation.

Related Topics
2.5 to 5-Axis Drilling Operations

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

    A Tapping entity is added to the Manufacturing Program. The Tapping 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 the red hole depth representation then select a threaded hole feature in the authoring window. 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.



    2. Select the axis representation in the sensitive icon to invert the tool axis direction, if required.

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

    • Approach clearance (A)
    • Depth mode: By shoulder (Ds): The depth value used is the one specified in the Geometry tab.
    • 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.

    See Specifying a Tool Element in a Machining Operation

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

    Note: in our example, the tool motion is as follows:


    • Motion at machining feedrate from 1 to 2
    • Reverse spindle rotation
    • Retract at machining feedrate from 2 to 3
    • Reverse spindle rotation

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

    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 Tapping 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

    The parameters available for PP word syntaxes for this type of operation are described in the NC_TAPPING section of the Manufacturing Infrastructure User's Guide.

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