Creating Machining Axis Systems

Create a Machining Axis System

You can create a machining axis system.

Click Machining Axis System .
The Machining Axis System dialog box opens. It contains a sensitive icon to help you define the origin and axis orientations.
By default, the X and Z axis are set to the corresponding directions of the absolute axis system. They are thus already defined and displayed in green.
Optional: Edit the proposed name.
This name is displayed beside the Machining Axis System in the work area.
Define the origin of the new Machining Axis System:
1. Click the dot representing the origin in the sensitive icon, then select a point or a circle in the work area.
  Alternatively, you can right-click the dot and select Coordinates to specify the coordinates of a point. Coordinates are expressed in the absolute axis system.
2. Select one of the axes in the sensitive icon to specify the orientation of that axis.
  See Defining the Tool Axis for more information.
3. Repeat the previous step for the next axis to define.
  Note: Since the Z axis is the privileged axis, we recommend that you define it first, then specify the X axis. The XY plane is perpendicular to the Z axis. The specified origin along with the X and Z axes thus are sufficient to define the Machining Axis System.
Alternatively: Click one or the triangular areas in the sensitive icon and select an existing axis system.
To analyze the geometry referenced by a Machining Axis System, right-click any sensitive area in the dialog box and select Analyze in the context menu
See Selecting Geometry for more information.
To specify an origin statement in the NC data output, select the Origin check box.
Depending on the machine type, specify an origin Number and Group.
For an origin with coordinates (0,0,0) and origin number and group both equal to 1, this results in the following type of output syntax:
```
$$*CATIA0 
         $$Origin.1 
         $$ 1.00000 0.00000 0.00000 0.00000	
         $$ 0.00000 1.00000 0.00000 0.00000	
         $$ 0.00000 0.00000 1.00000 0.00000
         ORIGIN/ 0.00000,0.00000,0.00000, 1, 1
```
Click OK.
The Machining Axis System is created in the Manufacturing View (Sort by Features).

Insert a Machining Axis Change

You can create a machining axis change.

From the Programming section of the action bar, click Machining Axis Change .
In the Machining Axis Change dialog box, define the origin of the new Machining Axis System.
See Creating Machining Axis Systems.
Select the PP Word Syntax tab .
See Inserting Post-Processor Instructions for more information.
Click OK.
The Machining Axis Change is added to the Activities Process Tree. In the Manufacturing View, it is created under a new Machining Axis System.
Notes:
- Machining Axis Changes do not impact the check reachability or table rotation. Similarly, the machine simulation is based on the toolpath and is not impacted by Machining Axis Changes.
- When table rotations are computed, the solution is provided with the least (that is, optimized) rotation.
- Output coordinates are computed in the current machining axis system as shown in the example below.
  The tool path is computed in the Machining Axis System AXS1 with origin (0,0,0):
  $$*CATIA0 $$*AXS1 $$ 1.00000 0.00000 0.00000 0.00000 $$ 0.00000 1.00000 0.00000 0.00000 $$ 0.00000 0.00000 1.00000 0.00000 GOTO/ -40.00000, -30.00000, 20.00000 GOTO/ -40.00000, 30.00000, 20.00000
  The same tool path is computed in the Machining Axis System AXS2 with origin (0,0,20):
  $$*CATIA0 $$*AXS2 $$ 1.00000 0.00000 0.00000 0.00000 $$ 0.00000 1.00000 0.00000 0.00000 $$ 0.00000 0.00000 1.00000 20.00000 GOTO/ -40.00000, -30.00000, 0.00000 GOTO/ -40.00000, 30.00000, 0.00000