Creating a Reverse Threading Operation with the Legacy Interface

You can create a Reverse Threading operation.

  1. From the Axial Machining section, select Reverse Threading then a position in the Manufacturing Program.
    • A Reverse Threading entity is added to the Manufacturing Program.
    • The Reverse Threading 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.
    1. Select the red hole depth representation then select a threaded hole feature.

      See Selecting Geometry

      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, if required.
    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 speeds for the operation.

    Example for 3 machining points:

    • Motion at machining feedrate from 1 to 2
    • Spindle off then reverse spindle rotation
    • Retract at machining feedrate from 2 to 3.

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

    See Defining and Editing Macros

  7. Click Tool Path Replay 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.
    Note: Boring bars are not supported during material removal simulation.
  8. Click OK to create the operation.
    Note: If your PP table is configured with the following statement for Reverse Threading 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_REVERSE_THREADING section of theNC Machining Apps Common Services User's Guide.

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