Create a Pocketing Operation
for Machining Closed Pockets

task target This task shows how to insert a Pocketing operation in the program when the pocket to be machined comprises hard boundaries only (that is, a closed pocket). 

To create the operation you must define:

  • the Pocketing mode as Closed Pocket
  • the tool that will be used
pre-requisites Open the PrismaticMilling01.CATPart document, then select Machining > Prismatic Machining from the Start menu. Make the Manufacturing Program current in the specification tree.  
scenario 1. Select Pocketing .

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

The Pocketing dialog box appears directly at the Geometry tab page . 
This tab page includes a sensitive icon to help you specify the geometry to be machined.

The bottom and flanks of the icon are colored red indicating that this geometry is required for defining the pocket.
All other pocket geometry is optional. 
Make sure that the Pocketing style is set to Closed Pocket.
2. Right click the red Bottom in the icon and select Contour Detection from the contextual menu.

Click the red Bottom then select the desired pocket bottom in the 3D window.

The pocket boundary is automatically deduced thanks to the Contour Detection setting. This is indicated by the highlighted Drive elements.
The bottom and flanks of the icon are now colored green indicating that this geometry is now defined.

For parts containing islands, you can right click the red Bottom in the icon and select Island Detection from the contextual menu. This allows island boundaries to be deduced automatically.
3. Click the Top Plane in the icon then select the desired top element in the 3D window.  
4. Set the following offsets:
  • 1.5mm on hard boundary
  • 0.25mm on bottom. 
If your part includes islands, you can specify different offsets on individual islands using the Offset on Island contextual command (right click the Island label in the 3D window).
5. Select the Strategy tab page and choose the desired tool path style: Inward helical, Outward helical or Back and forth.

You can then use the tab pages to set parameters for:
A tool is proposed by default when you 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.
6. Select the Feeds and Speeds tab page to specify the feedrates and spindle speeds for the operation.
7. Select the Macros tab page to specify the operation's transition paths (approach and retract motion, for example).
  • In the Macro Management frame, right-click the Approach line and select the Activate contextual command.
  • In the Current Macro Toolbox frame, select the Axial mode. A sensitive icon representing this approach motion is displayed. 
  • Double click the distance parameter in the sensitive icon and enter the desired value in the pop-up dialog box.

  • Repeat this procedure to specify the Retract motion.
See Define Macros of an Operation for another example of specifying transition paths on a machining operation. 
Before accepting the operation, you should check its validity by replaying the tool path.

8. Click OK to create the operation.

end of task