Creating a Boring Spindle Stop Operation with the Legacy Interface

You can create a Boring Spindle Stop operation.

  1. From the Axial Machining section, select Boring Spindle Stop then a position in the Manufacturing Program.
    • A Boring Spindle Stop entity is added to the Manufacturing Program.
    • The Boring Spindle Stop 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 hole geometry.

      See Selecting Geometry

      The sensitive icon is updated with information such as the number of machining points, the depth and diameter of the first selected hole, the hole extension type, ...

    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 specify the following machining 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.
    • Breakthrough (B) distance
    • Shift mode ( By linear coordinates or By polar coordinates).
    • Dwell mode (None, By revolutions, By time units).
    • Compensation parameters depending on those available on the tool.

    The other parameters are optional in this case.

  4. Select the Tool tab and choose a tool.

    Boring bar, boring and chamfering, end mill tools are supported.

    See Assigning a Tool Element to a Machining Operation.

  5. Select the Feeds and Speeds tab and specify the feedrates and spindle speeds for the operation.

    Example for 4 machining points:

    • 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 and Editing Macros

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

    Note: Boring bars are not supported during material removal simulation.

    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 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 NC Machining Apps Common Services User's Guide.

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