Turning on a Milling Center with Facing Head

task target This task illustrates how to create turning operations to machine large diameter holes on a milling center machine equipped with a facing head and rotary table. This is made possible by specifying local planes for turning at machining operation level.

The facing head is a mechanism mounted on the head of the milling center to support lathe tools. This configuration can be used to machine large diameter holes with better quality than milling.

In this scenario, the three large holes to be machined are located in different turning planes around the table rotary axis (C).

Each turning plane is defined by two axes (ZX) of a local machining axis system, so that each hole can be reached by rotating the table.

The tool mounted on the facing head is piloted along the U-axis to machine along the profile of the hole.

pre-requisites Open the TurningOperationOnMillMachine.CATProcess document, then select Machining > Lathe Machining from the Start menu.
scenario 1. Double-click the Part Operation and access the Machine editor. A 3-axis rotary table machine is already selected. Make the following settings in the Rotary Table tab.
2. Select the Machining Axis Change icon to create a local machining axis for the first hole.

Position the origin of the axis by selecting the outer circle of the hole. The axis origin will be positioned at the hole center.

Set the orientation of the X-axis (radial) and Z-axis (axial) by using one of the proposed methods (Selection or Manual Components, for example).
See Insert Machining Axis Change for more information about these methods.
3. Select the Profile Finish Turning icon .
Use the Geometry tab to:
  • Select the profile to machine making use of the sensitive Part Element symbol.
  • Specify the local plane making use of the sensitive axis system symbol.
    Select the local machining axis system that you created previously. The axial and radial axes (ZX) define the turning plane.

Use the Macro tab to define an approach macro by selecting a start point and a retract macro by selecting an end point.
 
  Use the Macro tab to define an approach macro by selecting a start point and a retract macro by selecting an end point.
Check the tool path by means of a replay.
   
  4. Repeat the steps above to create a local machining axis and a Profile Finish Turning operation for the other two holes.
   
  5. When the three turning operations are computed your program should look something like this:
     
  Please note the following points. They are dealt with in more detail in the Methodology section.
  • At each change of turning plane, you must define:
    • Machining Axis System Change: this is needed for NC data generation
    • Local machining axis system on turning operation: this is needed for processing geometry and visualizing the tool assembly.
  • NC data output can be generated in XYZ or XYZIJK format.
    For XYZ data, you must generate table rotations in your program.
    For XYZIJK data, the value that is output for IJK is taken on the Z axis (spindle) of the local machining axis system.
  • The following NC data statements will be generated at the start of each turning operation:
    • The coordinates of the origin of the local machining axis system
    • An order to switch from the X-axis to the U-axis.
      This is done through parameterized syntaxes in the PP table (NC_SPINDLE_LATHE or NC_LATHE_MO_START_COMMENT).

end of task