Creating a Chamfering Two Sides Operation

You can create a Chamfering Two Sides operation.

Related Topics
2.5 to 5-Axis Drilling Operations

  1. Activate the Manufacturing Program and click Chamfering Two Sides in the Axial Machining Operations toolbar.

    A Chamfering Two Sides entity is added to the Manufacturing Program.

    The Chamfering Two Sides dialog box appears directly at theGeometry 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 authoring window. Double-click to end your selections.



    2. Select the axis representation in the sensitive icon to invert the tool axis direction, if required.

  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 in seconds
    • 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. Go to the Tool tab to select a 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, tool motion is as follows:

    • 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 Macros on Axial Machining Operations

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

    Note: For material removal simulations, Two Sides Chamfering tools are not supported for Photo mode and are not collision checked in Video mode.

    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 Chamfering Two 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 Manufacturing Infrastructure User's Guide.

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