North America's Leading Siemens PLM Partner

Designfusion Blog

Using a Contour Surface Area operation to do undercutting

John Pearson - Thursday, May 21, 2015

Recently I had a customer contact me with a part that he wished to undercut. He needed to use a spherical cutter, which eliminated the Groove Milling operation, since it only uses T-cutters. Not being an advanced user he was unsure how to proceed. With his company’s permission I’ve decided to utilize this opportunity and create a blog article on how to use the Contour Surface Area operation to do undercutting.

Below is the image of the part along with the faces (highlighted in orange) that need to be machined.




Before creating the operation I need to generate some geometry to use as Drive and Projection geometry. First I create a small cylinder, protruded through the center of the part (shown below in magenta). This cylinder will be used for my drive geometry. In other words, I will initially create my tool paths on the cylinder and then project them onto the surface of the part.



I place this cylinder on an unused layer so I can easily hide and show it as needed. Next I create a line along the axis of the cylinder (shown below in yellow).



I place this line on an unused layer so I can easily hide and show it as needed. I will use this line to help project the paths from the drive geometry onto the surface of the part.


I then create my parent groups. For the Geometry group, the customer had created a WORKPIECE1 that contained the part and was a child to the MCS shown below. He’d also created the spherical mill for the Tool group, also shown below.




Along with the predefined PROGRAM and MILL_FINISH method I now have enough information to begin the operation.


I select the Contour Surface Area operation and assign the parent groups as shown below.



Once in the operation, my first step is to specify the cut area.



I click on the Specify Cut Area icon and select the faces that I wish to machine, as shown below.



Next I need to define the Drive Geometry. I select the Edit icon (small wrench) in the Drive Method section.



I then select the Specify Drive Geometry icon.



I turn on the layer that contains the previously created cylinder. Select the cylinder as shown below. Remember the surface will be used to create my initial tool paths.



I click OK to return to the Dive Method dialog. I then expand this dialog and set the drive settings and tolerances as required by the customer.



I can verify the results, of my drive geometry settings, by clicking the Display icon under the Preview heading. Notice the orange surface mesh representing my drive geometry.



Once I have my drive geometry created, I return to the main operation dialog to select my projection vector. To do this I first turn off the cylinder layer and turn on the line layer previously created. I then set the Projection Vector to Away from Line, as shown below.



I’m prompted to specify the Line/Vector, so I select the line that I had previously created. By doing this I’m telling the system to project the tool paths on the cylinder away from the axis towards the surface of the part.



Next I ensure that my Tool Axis is set to +ZM Axis.



I then modify the Engage motion, to use the center point of the opening, as shown below. This ensures that any engage motion will start in the center of the part.



I then set my Retract motion to match the Engage motion.



Finally I set my feeds and speeds to the required values, and then generate the operation. Notice the resulting undercut.




The Contour Surface Area operation allowed me to define how I was going to machine the cut area, by defining a cylindrical drive surface and projecting it away from an axial line, onto the cut area.


If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAM courses. To arrange for advanced training please contact your Account Manager, or contact us at [email protected].  


comments powered by Disqus