Create a Counterboring Operation with Legacy Interface

You can create a Counterboring operation.

  1. Activate the Manufacturing Program and click Counterboring in the Axial Machining action bar.

    A Counterboring entity is added to the Manufacturing Program.

    The Counterboring 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 3DEXPERIENCE platform. Double-click to end your selection.
      Closest, 1 point, Feature : Hole.33 (Counterbored), Diameter : 24mm, Depth : 30mm, Counterbore diameter : 34mm Counterbore depth : 10mm
    2. Select the axis representation in the sensitive icon to invert the tool axis direction, if required.
  3. Select theStrategy 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.
    • 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 Assigning a Tool Element to a Machining Operation

    You can use any of the following tool types:

    • End Mill
    • Drill
    • Multi Diameter Drill
    • Counterbore Mill
    • Countersink
    • Boring Bar
    • Boring and Chamfering tool
    • Reamer

  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, tool motion is at:
    • Motion at machining feedrate from 1 to 2
    • Dwell for specified duration
    • Retract at retract feedrate from 2 to 3.
  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.

    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 Counterboring operations: 
    CYCLE/CBORE, %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/CBORE, 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_COUNTERBORING section of the NC Machining Apps Common Services User's Guide.

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