Creating a Back Boring Operation

You can create a Back Boring operation.

Related Topics
2.5 to 5-Axis Drilling Operations

  1. Activate the Manufacturing Program and click Back Boring in the Axial Machining Operations toolbar.

    A Back Boring entity is added to the Manufacturing Program.

    The Back Boring 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 top plane representation then select the top of the part.
    2. Select the red hole depth representation then specify the hole pattern to be machined by selecting the two counterbored features in the authoring window.
    3. Double-click to end your selections.
    4. Select the axis representation in the sensitive icon to invert the tool axis direction, if required.

    The Geometry tab is updated with information about the first selected feature.



  3. Select the Strategy tab to specify the following machining parameters:

    • Approach clearance (A) and Approach clearance 2 (A2)
    • Depth mode: By tip (Dt)

      Note: The depth value used is the one specified in the Geometry tab.

    • Shift: By polar coordinates or By linear coordinates
    • Retract clearance
    • Compensation number depending on those available on the tool
    • Output CYCLE syntax.



  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:

    • Shift motion (if defined) at rapid feedrate from 1 to 2
    • Motion at rapid feedrate from 2 to 3
    • Shift motion (if defined) at rapid feedrate from 3 to 4
    • Motion at machining feedrate from 4 to 5
    • Dwell for specified duration
    • Retract clearance motion at retract feedrate from 5 to 6
    • Shift motion (if defined) at retract feedrate from 6 to 7
    • Retract at retract feedrate from 7 to 8
    • Shift motion (if defined) at retract feedrate from 8 to 9.

  6. Select theMacro 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.

    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.

    Note: For material removal simulations, Boring Bars are not supported for Photo mode and are not collision checked in Video mode.

  8. Click OK to create the operation.

    Note: If your PP table is customized with the following statement for Back Boring operations:

    CYCLE/BORE, %MFG_TOTAL_DEPTH, %MFG_FEED_MACH_VALUE,
&MFG_FEED_UNIT,%MFG_CLEAR_TIP, ORIENT, %MFG_XOFF, DWELL, %MFG_DWELL

    A typical NC data output is as follows:

    CYCLE/BORE, 25.000000, 500.000000, MMPM, 5.000000, ORIENT,
1.000000, DWELL, 3

    The parameters available for PP word syntaxes for this type of operation are described in the NC_BACK_BORING section of the Manufacturing Infrastructure User's Guide.

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