Multi-Axis Curve Machining: Contact

task target This task shows how to insert a 'Contact' Curve Machining operation in the program. To create the operation you must define:
  • the Curve Machining mode as Contact
  • the tool that will be used
  • the parameters of the machining strategy with the tool axis guided in Lead and Tilt mode


You can modify the parameters of two or more Multi-Axis Curve Machining operations in one shot by means of the Selected Objects > Definition... contextual command.
Editing Parameters of Several Multi-Axis Curve Machining Operations.

pre-requisites Open the MultiAxisMilling01.CATPart document, then select Machining > Advanced Machining from the Start menu. 
Make the Manufacturing Program current in the specification tree.  
  1. Select the Multi-Axis Curve Machining icon .
    The Multi-Axis Curve Machining dialog box appears directly at the Geometry tab page
    This page includes a sensitive icon to help you specify the geometry to be machined.
    Set  the Curve Machining mode to Contact to drive the contact point.
    The part and guide curve in the icon are colored red indicating that this geometry is required for defining the operation.
    All other geometry is optional. 

  2. Click the red part in the icon, then select the four faces in the 3D window as shown in the figure below.

  3. Click the red guide element  in the icon, then select four edges in the 3D window as shown in the figure below.
    Note that a Guide is created for each set of continuous edges, and that discontinuous Guides are accepted.
    The four faces and the four edges are selected:

The part and guide elements of the icon are now colored green indicating that this geometry is now defined.
These are also indicated on the part. Make sure that the arrows representing the part surface orientation are all pointing upwards.
  1. Select the Strategy tab page . You can then use the tab pages to set parameters for:

    • Tool Axis 
      Specify Fixed Lead and Tilt with Lead angle = 20deg and Tilt angle = 0deg.
A tool is proposed by default when you want to create a machining operation. 
If the proposed tool is not suitable,  just select the Tool tab page to specify the tool you want to use.
This is described in Edit the Tool of an Operation.
  1. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.

If you want to specify approach and retract motion for the operation,
select the Macros tab page to specify the desired transition paths.
If a transition between two curves is smaller than the tool diameter, the clearance macro is not executed.
The tool continues straight on over the gap between the curves.
The general procedure for this is described in Define Macros of an Operation.
  1. Check the validity of the operation by replaying the tool path.

  2. Click OK to create the operation.

end of task