Creating a Thread Milling Operation

You can create a Thread Milling operation. For this operation, machining is done in one or more helical passes.

This task shows you how to:

Creating a Thread Milling Operation

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

    The Thread Milling 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 Thread Milling entity is added to the Manufacturing Program.

    The Thread Milling 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 ThreadMilling.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.
    • 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 thread milling operation is created as ThreadMilling.x. It is visible in the Activities Process Tree.

Creating a Thread Milling Operation with the Legacy Interface

  1. From the Axial Machining section, select Thread Milling then a position in the Manufacturing Program.
    • A Thread Milling entity is added to the Manufacturing Program.
    • The Thread Milling 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 the threaded 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.
    3. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.
  3. Select the Strategy tab and set the following parameters:
    • Machining Strategy (Mono pass or Optimized pass)
    • Machining Direction (Top to bottom or Bottom to top)
    • Approach clearance (A)
    • Breakthrough (B)
    • Machining tolerance
    • Plunge mode (None or By tip)
    • Compensation number depending on those available on the tool.
    The tool path representation displayed in this tab varies according to the Machining strategy and Machining direction.
  4. Select the Tool tab and choose a tool.

    Thread mill and boring bar tools are supported.

    See Assigning a Tool Element to a Machining Operation.

    Notes:
    • Boring bar tools support only Mono-pass machining.
    • When optimizing passes with a thread mill too, the number of helical tool paths depends on the effective thread length of the tool and the thread depth of the hole.

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

    Example for 5 machining points:

    • Motion at machining feedrate from 1 to 2
    • Motion at feedrates defined on macros from 2 to 3 and 3 to 4
    • Retract at retract feedrate from 4 to 5.

  6. Select the Macros tab to specify the operation transition paths (approach and retract motion, for example).

    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 Thread Milling 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_THREAD_MILLING section of the NC Machining Apps Common Services User's Guide.

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