Creating a Drilling Deep Hole Operation

You can create a Drilling Deep Hole operation.

Related Topics
2.5 to 5-Axis Drilling Operations

  1. Activate the Manufacturing Program and click Drilling Deep Hole in the Axial Machining Operations toolbar.

    A Drilling Deep Hole entity is added to the Manufacturing Program.

    The Drilling Deep Hole 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 features as shown below. 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 to specify the following 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
    • Maximum depth of cut (Dc) and Retract offset (Or)
    • Decrement rate and Decrement limit
    • Dwell mode
    • 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.

    You can make use of the hole diameter found on the selected hole feature to select an appropriate tool.

    See Specifying a Tool Element in a Machining Operation

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

    Note: In the tool path represented in the Strategy tab,

    • The tool motion is as follows:
      • Motion at machining feedrate from 1 to 2
      • Dwell for specified duration
      • Retract at retract feedrate from 2 to 3
      • Motion at plunge feedrate from 3 to 4
      • Motion at machining feedrate from 4 to 5
      • Dwell for specified duration
      • Retract at retract feedrate from 5 to 6
      • Motion at plunge feedrate from 6 to 7
      • Motion at machining feedrate from 7 to 8
      • Dwell for specified duration
      • Retract at retract feedrate from 8 to 9.
    • Distance (1,2) = A + Dc Distance (3,4) = A + Dc - Or Distance (4,5) = Or + Dc*(1 - decrement rate) Distance (7,8) = Or + Dc*(1 - 2*decrement rate).
    • Depth of current peck > Maximum depth of cut * Decrement limit.

    For more information, see Example of Decrement rate and Decrement limit.

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

    See Defining Macros on Axial Machining Operations

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

    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 Drilling Deep Hole operations: 

    CYCLE/DEEPHL, %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/DEEPHL, 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_DEEPHOLE section of the Manufacturing Infrastructure User's Guide.

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