Creating a Chamfering 2 Sides Operation with Legacy Interface

You can create a Chamfering 2 Sides operation.

  1. From the Axial Machining section, select Chamfering 2 Sides then a position in the Manufacturing Program.
    • A Chamfering 2 Sides entity is added to the Manufacturing Program.
    • The Chamfering 2 Sides 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, ...

    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) and Approach clearance 2 (A2)
    • Depth mode (By tip (Dt))
    • Dwell mode (None, By revolutions, By time units) and the corresponding values.
    • First compensation number depending on those available on the tool for top chamfering
    • Second compensation number depending on those available on the tool for bottom chamfering.

    Note: The depth value and chamfer diameter are retrieved from your geometry selections.

  4. Select the Tool tab and choose a tool.

    Two sides chamfering 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 5 machining points:

    • Motion at machining feedrate from 1 to 2
    • Dwell for specified duration
    • Possibly, activation of second tool compensation number (output point change)
    • Motion at approach feedrate from 2 to 3
    • Motion at machining feedrate from 3 to 4
    • Dwell for specified duration
    • Possibly, activation of first tool compensation number (output point change)
    • Retract at retract feedrate from 4 to 5.

  6. Select the Macro tab to 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 Chamfering 2 Sides operations:
    CYCLE/BORE, %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/BORE, 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_TWO_SIDES_CHAMFERING section of the NC Machining Apps Common Services User's Guide.

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