Creating a Boring Spindle Stop Operation

You can create a Boring Spindle Stop operation.

Related Topics
2.5 to 5-Axis Drilling Operations

  1. Activate the Manufacturing Program and click Boring Spindle Stop in the Axial Machining Operations toolbar.

    A Boring Spindle Stop entity is added to the Manufacturing Program.

    The Boring Spindle Stop 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 the hole geometry in the authoring window. Double-click to end your selections.

      The sensitive icon is updated with the following information:

      • depth and diameter of the first selected hole
      • hole extension type: through
      • number of points to machine.


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

  3. Select the Strategy tab and specify the following machining parameters:

    • Approach clearance (A)
    • Depth mode: By tip (Dt)

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

    • Breakthrough (B) distance
    • Shift mode: By linear coordinates or By polar coordinates.
    • Dwell
    • 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 and specify the feedrates and spindle speeds for the operation.

    Note: In the tool path represented in the Strategy tab, tool motion with a boring bar is as follows:

    • Motion at machining feedrate from 1 to 2
    • Dwell for specified duration
    • Spindle stop
    • Shift motion at retract feedrate from 2 to 3
    • Retract at retract feedrate from 3 to 4
    • Shift motion at retract feedrate from 4 to 1.

  6. Select the Macro tab and add approach and retract motions to the operation.

    See Defining Macros on Axial Machining Operations

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

    Note: For material removal simulations, Boring Bars are not supported for Photo mode and are not collision checked in Video mode.

    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 Boring Spindle Stop operations: 

    CYCLE/BORE, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
&MFG_FEED_UNIT,%MFG_CLEAR_TIP, ORIENT, %MFG_XOFF, DWELL, %MFG_DWELL_REVOL

    A typical NC data output is as follows: 

    CYCLE/BORE, 25.000000, 500.000000, MMPM, 5.000000, ORIENT,
1.000000, DWELL, 3

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

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