Create a Groove Milling Operation

task target This task shows how to insert a Groove Milling operation in the program. To create the operation you must define:
  • the tool that will be used
pre-requisites Open the sample_groove_milling.CATPart document, then select the desired Machining workbench from the Start menu. Make the Manufacturing Program current in the specification tree.  
scenario 1. Select Groove Milling . The Groove Milling dialog box appears directly at the Geometry tab page . This page includes a sensitive icon to help you specify the geometry to be machined.
The groove top, bottom and flank in the icon are colored red indicating that this geometry is required for defining the operation. All other geometry is optional. 

Note that Contour Detection contextual command is not activated.
2. Click the red bottom in the icon, then select the bottom of the groove in the 3D window.
3. Click the red top in the icon, then select the top of the groove in the 3D window.
4. Click the red guiding element in the icon, then select the flank contour of the groove in the 3D window.
  If the Contour Detection contextual command is set, the boundary of the selected face will be proposed automatically as guiding contour. See Specifying Guiding Contours for more information.
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.
Set the Offset on Limit1 to 5mm.
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.
Set the Offset on Limit2 to 5mm.

See Specifying Relimiting Elements for more information.
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.

7. Select the Strategy tab page and choose the desired tool path style. You can then use the tabs to set parameters for:
8. 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.
9. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
10. Check the validity of the operation by replaying the tool path.
   
   
The specified operation uses a default Return between levels macro to allow switching compensation points for machining upper and lower levels of the groove.

You can optimize this macro and add approach and retract macros to the operation in the Macros tab page . This is described in Define Macros of a Milling Operation.
11. Click OK to create the operation.
  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