CATIA surface with sawtooth edge

Jack K

8 Dec, 2020 01:42 PM

Step-by-step instructions for how to make a sawtooth pattern on a curved surface, using a CATIA Law.

(This chevron pattern is used on engine cowlings to reduce noise)

1. Step 1: Start with a surface

   Start with a surface. A simple revolved surface will work for this tutorial. It can be a simple cylinder or cone, or a barrel shape like below. It doesn't have to be revolved - any surface will work.

   
   

   Split the surface in half, so it only contains 180° of rotation. When we're done, we can do a mirror operation to get the entire shape.

   

2. Step 2: Add a reference curve

   We need a reference curve to locate the sawtooth pattern.

   
   

   Add a plane near the end of the surface, and intersect the surface with the plane to get the reference curve.

   
   

   Measure the curve to find the approximate length. (the curve below is 6.345 long, or approx 6.0)

   

3. Step 3: Define the sawtooth

   Now we get to draw the sawtooth. For this tutorial, we'll keep it simple and just draw 4 teeth.

   
   

   A. Make a Sketch, like the one below.

   
   

   
   

   1. start with a horizontal line, and make it about the same length as the reference curve we measured before.
   2. change this line to Construction.
   3. draw the zig-zag pattern of the sawtooth. (I just drew 2 lines for the first tooth, and then translated to get the others)
   4. If you want, you can round-off the corners or make the sawtooth more complex. Just make sure you have a single profile before you exit the sketch

   

   B. EXIT the sketch

   
   

   C. Then, draw a line from the beginning vertex of the sawtooth to the ending vertex, just like the purple line below:

   

   
   

   D. Add a Law:

   1. click the Law icon (or click Insert in the top menu, slide down and click Law, and slide right and click the Law command)
   2. click the purple line for the Law Reference
   3. click the sketch for the Law Definition
   4. and click OK to make the Law (it should appear in the tree)

   

   
   

   
   

4. Step 4: Wrap the sawtooth onto the Surface

   Add a Parallel Curve:

   
   

   
   

   1. click the Parallel Curve icon
   2. click the Intersection curve to be the reference
   3. click the surface to be the support
   4. instead of keying a constant value, click on the Law... button
   5. select Law.1 in the tree
   6. a little pop-up appears with a preview of the wrapped sawtooth. Close the pop-up window
   7. If necessary, click the red arrows to flip the direction of the sawtooth
   8. click OK to add the Parallel Curve "wrapped" onto the surface

   

   
   

   Notice how the 3D sawtooth curve has been scaled to match the exact length of the intersection curve.

5. Step 5: Trim the surface

   A. Split the surface using the Parallel curve as the cutting element

   

   
   

   B. Mirror the surface about the center plane to obtain the whole surface

   

   
   

   
   

6. Step 6: The final solid version

   Join the two surface halves together. Then switch to the Part Design workbench and use the Surface Thickness command to make a solid from the surface.

   Add more features, such as Fillets, Holes, and Material.

   You can always go back and modify the sketch to change the sawtooth pattern.

   

   I hope I taught you something. Please leave a comment and let me know what you think. Thanks