Creating a Reaming Operation with Legacy Interface

You can create a Reaming operation.

Before you begin: Create a machining pattern as explained in Defining Machining Patterns.
  1. From the Axial Machining section, select Reaming then a position in the Manufacturing Program.
    • A Reaming entity is added to the Manufacturing Program.
    • The Reaming 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, select a machining pattern from the New Pattern list.
    1. Optional: Select the axis representation in the sensitive icon to invert the tool axis direction.
    2. 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, the hole extension type, ...

  3. Select the Strategy tab to specify the following parameters:
    • Approach clearance (A)
    • Depth mode (By tip (Dt) or By shoulder (Ds))
      Note: The depth value used is the one specified in the Geometry tab.
    • Dwell mode (None, By revolutions, By time units) and the corresponding values.
    • Compensation parameters 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

  5. Select the Feeds and Speeds tab to specify the feedrates and spindle speeds for the operation.

    Example for 3 machining point:

    • Motion at machining feedrate from 1 to 2
    • Dwell for specified duration
    • Retract at retract feedrate from 2 to 3.

  6. Select the Macros tab to specify the desired transition paths.

    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 Reaming operations: 
    CYCLE/REAM, %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/REAM, 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_REAMING section of the NC Machining Apps Common Services User's Guide.

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