Create a Sequential Groove Machining Operation

task target This task shows how to insert a Sequential Groove operation in the program. 

To create the operation you must define:

  • the tool that will be used

Please refer to Sequential Axial and Sequential Groove Operations in the Reference section for detailed information about this operation.
pre-requisites Open the Sequential_Groove.CATPart document, then select Machining > Prismatic Machining from the Start menu. Make the Manufacturing Program current in the specification tree. 

scenario 1. Select Sequential Groove  .

A Sequential Groove entity along with a default tool is added to the program.

The Sequential Groove dialog box appears directly at the Geometry tab page .

    The Global tab allows you to define the hole geometry to machine.
  2. Select the red groove depth representation in the sensitive icon, then select the two holes in the part.
Set the Number of levels to 2.
Just double click to end your selections.

  3. Select the Local tab to define the machining planes to reach.
For Level number 1, select the plane representations in the sensitive icon, and the planes of the first groove in the part.
The Local tab is updated as shown below.

For Level number 2, select the appropriate planes of the second groove in the part.
4. Select the Tool tab page to replace the default tool by a more suitable one.

Select a T-slotter tool and set the nominal diameter to a value less that 40mm (so that the tool can pass through the top of the hole).
Select the Compensation tab and specify a second corrector P2 as follows:

See Edit the Tool of an Operation for more information about selecting tools.
  5. Select the Strategy tab page , which comprises two tabs Motions and Strategy.
The Motions tab allows you to define the elementary motions making up the machining operation.
6. Click Go to Plane , then define a Goto a plane motion to Plane 1 and a local feedrate of 50mm/mn. Set Compensation to 2.

Click OK to add the first tool motion in the list in the Sequential Groove dialog box.
7. Click Circular , the define a circular motion.

Note that you may need to adjust the radius of the circular approach (and circular retract) portion of this motion to be compatible with the groove and tool radius values.
Just right-click the circular arc in the icon, and set the radius parameter to 5mm.

Click OK to add the motion in the list.
8. Click Go to Plane , the define a Goto a plane motion to Plane 2 and a local feedrate of 50mm/mn. Set Compensation to 1.

Click OK to add the tool motion in the list.
9. Insert other motions as follows:
  • Circular motion at machining feedrate
  • Go to Clearance motion with local feedrate of 500mm/mn.
    Right-click this motion in the list and set the Application mode to Last level.
   
10. Select the Strategy tab to specify machining parameters such as Approach clearance.
Make sure the Compensation application mode is set to Guiding Point.
11. If needed, select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
12. If you want to specify approach and retract motion for the operation, select the Macros tab page to specify the desired transition paths. 
The general procedure for this is described in Define Macros of an Operation.
  13. Check the validity of the operation by replaying the tool path.

14. Click OK to create the operation.

end of task