Creating a Drilling Break Chips Operation with the Legacy Interface

You can create a Drilling Break Chips operation.

  1. From the Axial Machining section, select Drilling Break Chips then a position in the Manufacturing Program.
    • A Drilling Break Chips entity is added to the Manufacturing Program.
    • The Drilling Break Chips 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 feature.

      See Selecting Geometry for more information.



      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 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
    • Maximum depth of cut (Dc) and Retract offset (Or)
    • Dwell mode (None, By revolutions, By time units) and the corresponding values.
    • 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.

    Drill, spot drill, center drill, multi diameter drill, end mill 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 7 machining points:

    • Motion at machining feedrate from 1 to 2
    • Dwell for specified duration
    • Retract at retract feedrate from 2 to 3
    • Motion at machining feedrate from 3 to 4
    • Dwell for specified duration
    • Retract at retract feedrate from 4 to 5
    • Motion at machining feedrate from 5 to 6
    • Dwell for specified duration
    • Retract at retract feedrate from 6 to 7
    • Distance (1,2) = A + Dc Distance (2,3) = Distance (4,5) = Or Distance (3,4) = Distance (5,6) = Or + Dc.

  6. Select the Macro tab and specify the desired transition paths.

    See 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 Drilling Break Chips operations: 
    CYCLE/BRKCHP, %MFG_TOTAL_DEPTH, INCR, %MFG_AXIAL_DEPTH,
 %MFG_FEED_MACH_VALUE, &MFG_FEED_UNIT,
 %MFG_CLEAR_TIP, DWELL, %MFG_DWELL_REVOL

    A typical NC data output is as follows: 

    CYCLE/BRKCHP, 25.000000, INCR, 5.000000, 500.000000, MMPM,
5.000000, DWELL, 3

    The parameters available for PP word syntaxes for this type of operation are described in the NC_BREAK_CHIPS section of the NC Machining Apps Common Services User's Guide.

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