Turning on a Milling Center with Facing Head

This section provides information about creating turning operations on a 3-axis milling machine that is equipped with a rotary table and facing head. The main objective is to machine large diameter holes using turning techniques, which will give better quality results than milling.

In particular, this section explains how to:

Set Up the Part and Machining Environment

The Part Operation editor allows you to set up the part and the machining environment.

Define the Reference Machining Axis System

Click Reference Machining Axis System . The Machining Axis System dialog box appears for assigning a reference machining axis system to the part operation. This is similar to the procedure described in Insert Machining Axis Change.

The coordinates of the NC output data will be expressed in this axis system. However, when a local machining axis system is inserted in the program, coordinates will be expressed in the local axis system.

The reference machining axis system should be positioned such that it is Y-axis is collinear with the rotary axis of the machine (B).

Assign the Part to be Machined

Click Product to associate the part to machine (CATProduct or CATPart) to the part operation.

Other important parameters to set in the Part Operation Editor are:

Select the Machine and Set Parameters

Click the Machine icon then select the 3-axis with Rotary Table Machine type in the Machine Editor.

In the case of an actual machine with facing head on the shop floor, the XYZIJK output could be post-processed to pilot the U-axis of the facing head.
The tool mounted on the facing head machines along the profile of the hole.
Note that this information is not specified in the Machine Editor dialog box.

In the Numerical Control tab, select the following sample PP word table is delivered with the product in

Other important parameters to set in the Machine Editor are:

Define Local Machining Axis Systems and Turning Planes

If you specify turning operations on a milling machine, they will be described in the ZX turning plane of the reference machining axis system.

To specify turning operations on a milling machine equipped with a facing head and rotary table, you must define local machining axis systems. Local turning planes will be derived from the Z and X axes of these axis systems. The geometry to machine must lie in the turning plane in order to create the turning operations.
The figure below shows a local machining axis system with the ZX turning plane and the selected geometry (Part Element in red) that lies in this plane.

Therefore at each change of turning plane, you must define a local machining axis for turning operations. This is needed for processing geometry and visualizing the tool assembly.

Methodology: Machining Axis Changes or Table Rotations

Using Machining Axis Changes

To output NC data in the axis system defining the local plane, you must define a Machining Axis System Change before each turning plane.

A typical program is shown in the figure below:

When NC data is generated in XYZIJK format, the IJK components will be the Z-axis of the local plane (see NC Data Output for more information).

Using Table Rotations

Define your turning operations in the corresponding local axis systems, then generate Machine Rotation instructions in the program using the command Generate Machine Rotation command.

A typical program is shown in the figure below:

When NC data is generated in XYZIJK format, the IJK components will be the Z-axis of the local plane (see NC Data Output for more information).

Replay and Simulation

You should replay the tool path to check each operation.

You should simulate the material removed by the program. You will need to specify design part and stock in the Part Operation editor.

NC Data Output

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:





A typical APT output would be:

$$ OPERATION NAME : Profile Finish Turning.1
$$ Start generation of : Profile Finish Turning.1
LOCAL_ORIGIN, 0.00000, 130.00000, 0.000000
SPINDL/ 70.0000,RPM
GOTO / ...

Some Points to Note 

The Update Input Stock capability is not available for turning operations on milling centers. The corresponding commands are not available in the Part Operation or Turning Operation editors.