Create a Profile Contouring Operation
Between Two Planes

task target This task shows how to insert a 'Between Two Planes' Profile Contouring operation in the program.

To create the operation you must define:

  • the Contouring mode as Between two planes
  • the tool that will be used
pre-requisites Open the PrismaticMilling01.CATPart document, then select the desired Machining workbench from the Start menu. Make the Manufacturing Program current in the specification tree. 
scenario 1. Select Profile Contouring I_MfgProfileContouring.gif (963 bytes). The Profile Contouring 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 Contouring mode to Between Two Planes.
The part bottom and flanks 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 bottom in the icon, then select the underside of the part in the 3D window.
3. Set the Bottom type to Soft by clicking the text, then set the Offset on Bottom to -5mm.
4. Click the red flank in the icon, then select the profile along the front edge of the part in the 3D window.
5. Right click Start to set this condition to Out.

Click the first relimiting element in the icon, then select the horizontal edge at one end of the contour profile in the 3D window.
6. Right click Stop to set this condition to Out.

Click the second relimiting element in the icon, then select the horizontal edge at the other end of the contour profile in the 3D window.
7. Click the check element in the icon, then select the top face of the green fixture in the 3D window.
The bottom, guide, limit and check elements of the icon are now colored green indicating that this geometry is now defined. These are also indicated on the part.

8. Select the Strategy tab page and choose the desired tool path style. You can then use the tabs to set parameters for:

Output type in the Machining tab allows you to manage the generation of Cutter compensation (CUTCOM) instructions in the NC data output. See Reference section for more information.
9. 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.
10. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
11. Check the validity of the operation by replaying the tool path.

The specified operation uses a default linking macro to avoid collision with the selected fixture.

You can optimize the linking macro and add approach and retract macros to the operation in the Macros tab page .

Please note that if a user-defined linking macro is not collision free, a default linking macro is applied.

For more information please refer to Define Macros of a Milling Operation.
12. Click OK to create the operation.
 

More About Profile Contouring Operations

Multi-Edition

You can modify the parameters of two or more Profile Contouring operations in one shot by means of the Selected Objects > Definition...  contextual command. See Editing Parameters of Several Profile Contouring Operations.

Collision Checking

A Collision Checking capability is available in the Geometry tab page, which allows collision checking between the tool and guide elements during macro motions. See Reference section for more information.

end of task