Creating a Tapping Operation

You can create a Tapping operation.

This task shows you how to:

Creating a Tapping Operation

  1. From the Axial Machining section of the action bar, select Tapping , then select a position in the manufacturing program.

    The Tapping workflow appears in the work area.

  2. In the Tool Search dialog box that appears:
    1. Select the tool type.
    2. Select the required tool or tool assembly and click one of the following:
    OptionDescription
    Select in Session Select an existing tool or tool assembly from the Resource Configuration View.
    Search in Database Select a tool or a tool assembly from the database.
    Look Into Catalog Browse for a tool or a tool assembly in the catalog.
  3. Optional: Close the Tool Search dialog box by pressing Esc. Then, click Search Tool to research a tool in the database.
  4. Follow the workflow instructions to select hole positions, or select an existing manufacturing pattern from the Manufacturing View.
  5. Double-click anywhere in the work area.

    A Tapping entity is added to the Manufacturing Program.

    The Tapping dialog box appears directly in the Geometry tab .

  6. Click in the title bar of the dialog box to edit the name of the manufacturing pattern, such as Tapping.x.
  7. Optional: Click New Feature to apply a machining area feature.

    Note: You can export a feature by clicking Export Feature .

  8. In the Mandatory section, verify the mandatory input parameters.

    Note: The following icons are used to describe the status of a parameter:
    Icon Description
    Parameter defined.
    Mandatory parameter not defined.
    Optional parameter not defined.
    Parameter not up to date.
    Broken link.

  9. Optional: Do any of the following:
    1. Click to remove the input parameter.
    2. Click to display additional information on the parameter in the work area.
    3. Click to display the parameter's context menu.
  10. In the Optional section, verify the optional input parameters.
  11. In the Parameters section, verify additional parameter inputs.
  12. Verify the parameters in the following tabs:

    • Tool: Select a tool.
    • Strategy: Select a Tool path style and Tapping Mode: Tapping, Reverse Threading, or Thread with TapHead.
    • Feeds and Speeds: Specify the feedrates and spindle speed.
    • Macros: Specify transition paths.

  13. Click Edit Cycle to edit or choose output syntaxes.
  14. Click Compute to compute the tool path with the specified parameters.
  15. Click OK to validate and exit the dialog box.
  16. Click Cancel to exit the dialog box without saving.

The tapping operation is created as Tapping.x. It is visible in the Activities Process Tree.

Creating a Tapping Operation with the Legacy Interface

  1. From the Axial Machining section, select Tapping then a position in the Manufacturing Program.
    • A Tapping entity is added to the Manufacturing Program.
    • The Tapping dialog box opens directly at the Geometry tab . This tab includes a sensitive icon to help you specify the geometry.
    • Areas colored red, texts such as No point and No geometrical feature has been selected indicated that 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.

      See Selecting Geometry for more information.

      The sensitive icon is updated with information such as the thread pitch, direction, depth and diameter, hole extension type, number of machining points, ...
    2. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
    3. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
  3. Select the Strategy tab to specify the following parameters:
    • Approach clearance (A)
    • Depth mode (By tip (Dt) or By shoulder (Ds))
      Note: 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. Select the Tool tab and choose a tool.

    Tap tools are supported.

    See Assigning a Tool Element to a Machining Operation.

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

    Example for 3 machining points:

    • 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 and Editing Macros

  7. Click Display or Simulate to check the validity of the operation.

    See Simulating 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 configured 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 NC Machining Apps Common Services User's Guide.

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