Creating a Back Boring Operation with the Legacy Interface

You can create a Back Boring operation.

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

      See Selecting Geometry for more information.

    3. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
    4. Optional: Select the check boxes below the sensitive icon to modify the corresponding data.

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

  3. Select the Strategy tab to specify the following machining parameters:
    • Approach clearance (A) and Approach clearance 2 (A2)
    • Depth mode (By tip (Dt) or By shoulder (Ds))
      Note: The depth value used is the one specified in the Geometry tab.
    • Shift mode (None, By polar coordinates or By linear coordinates
    • Retract clearance
    • Dwell mode (None, By revolutions, By time units).
    • Compensation parameters depending on those available on the tool
    • Automatic ROTABL
    • Output CYCLE syntax.
  4. Select the Tool tab and choose a tool.

    Boring bar, 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 9 machining points:

    • 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 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.
    Note: Boring bars are not supported during material removal simulation.
  8. Click OK to create the operation.
    Note: If your PP table is configured 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 NC Machining Apps Common Services User's Guide.

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