Creating a Drilling Dwell Delay Operation with the Legacy Interface

You can create a Drilling Dwell Delay operation.

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

      See Selecting Geometry for more information.



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

    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 to 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.
    • Dwell delay
    • Compensation number depending on those available on the tool.

    The other parameters are optional in this case.

  4. Select the Tool tab and choose a tool.

    Tip: Use the hole diameter found on the selected hole feature to select the appropriate tool.

    Drill, spot drill, center drill, multi diameter drill, countersink, boring and chamfering, boring bar, reamer and 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 3 machining points:

    • Machining feedrate from 1 to 2
    • Dwell for the specified duration
    • Retract or rapid feedrate from 2 to 3.

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

    See Defining and Editing Macros

  7. Click Tool Path Replay 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 Dwell Delay operations: 
    CYCLE/DRILL, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
&MFG_FEED_UNIT,%MFG_CLEAR_TIP, DWELL, %MFG_DWELL_REVOL

    A typical NC data output is as follows: 

    CYCLE/DRILL, 25.000000, 500.000000, MMPM, 5.000000, DWELL, 3

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

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