Inserting Machining Axis Changes

task target This task shows how to add machining axis changes in the program.

Output coordinates are computed in the current machining axis system as shown in the example below.

Tool path computed in 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

Same tool path computed in 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
pre-requisites Either the program or a program entity must be current in the specification tree.
scenario 1. Select Machining Axis Change in the Auxiliary Operations toolbar.

The corresponding dialog box is displayed directly at the Geometry tab .

The X and Z axes are shown already defined (green) because, by default, they are set to the corresponding directions of the absolute axis system. You can define a new machining axis system by specifying new axis orientations as described below.

You can define your axis system with the help of the sensitive icon in the dialog box. 
2. In the Axis name field, you can enter a name for the machining axis system being created. This name will be displayed beside the representation of the axis system in the 3D view. 
3. Select the symbol representing the origin in the sensitive icon, then select a point or a circle to define the origin of the machining axis.
  In addition to point selection, you can also specify a point by means of its coordinates as follows:
  • right-click the symbol representing the origin in the sensitive icon
  • select the Coordinates contextual command
  • enter the point coordinates in the dialog box that appears.

Coordinates are expressed in the absolute axis system.

4. Select one of the axes (Z, for example) in the sensitive icon to specify the orientation of that axis. 

The following dialog box appears.
The Z axis is the privileged axis. You should define it first, then specify the X axis. The XY plane is perpendicular to the Z axis.
5. Select the desired method to specify the axis orientation in the proposed list:
  • Manual. In this case, choose one of the following:
    • Components to define the orientation by means of I, J and K components
    • Angles to define the orientation by means of a rotation specified by means of one or two angles:
      Angle 1 about X, Angle 2 about Y
      Angle 1 about Z, Angle 2 about X
      Angle 1 about Y, Angle 2 about Z
  • Selection. In this case just select a line or linear edge to define the orientation.
  • Points in the View. In this case just select two points to define the orientation.

Just click OK to accept the specified orientation.
6. Repeat this procedure to specify the orientation of another axis (X, for example).

The specified origin along with the X and Z axes are sufficient to define the machining axis system.
You can also define a machining axis by selecting one of the triangular areas in the sensitive icon.  In this case you must select an existing axis system and position it by selecting a point in the 3D view.
7. You can select the Origin check box if you want to specify an origin statement in the NC data output.

For certain machine types it may be useful to specify an origin number and group. This will result 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

This output is for an origin with coordinates (0,0,0) and whose origin number and group are both equal to 1.  
8. Select the Syntax tab .
  • Select the Initialize from PP words table check box to consult the Machining Axis Change syntax defined in the PP table that is referenced by the Part Operation.
  • Otherwise, enter a PP instruction for your machining axis change. This user-defined syntax has no link with the PP table and its validity is not checked by the program.
9. Click OK to create the machining axis change in the program. A feature representation of the corresponding Machining Axis System is created in the 3D view.
  Please note the following:
  • It is possible to analyze the geometry referenced by a machining axis system. This geometry may be a point, line, surface, or an axis defined in the design part. Right-click any sensitive area in the dialog box, and select Analyze. The Geometry Analyser dialog box appears giving the referenced geometry, its name and status.
  • A machining axis system can be shared by several machining axis change operations. Machining axis systems can be listed in Manufacturing View using the Sort by Features command.

end of task