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Modeled in Creo Parametric 7.0.0.0, we need to wrap, offset with expand feature option, pattern, remove and reference pattern options....will work on the cylinder cam example and update you....Its possible in Creo but not as straightforward as SolidWorks!

thank you and I'll wait for your update for the cylinder cam, I'm going to try make it following your steps.

I got the desired result using wrap and sweep cut in Creo, not sure why you are not getting the desired output with wrap for this part.

Used Surfacing Technique. Wrap the curve. Copy External Surfaces. Trim copied surface one way. Trim copied surface another way. Thicken the resultant surface with a cut.

Might be a way to do it with a sweep if I can control the x-direction.

O thanks Enrique for your input, I think you're method is the best one because I made it like Mr. Rasesh Palav (wrap & sweep cut) but even in his model images you can see the bottom surface of the curve with the smallest radius (inner) lifted up or deformed and I'm sure that on the sides the depth of the cut is different than on the front and back. If you Mr. Palav can make a several section views at a different distances and in the horizontal and vertical directions just to see if the depth of cut is constant & the bottom surface is uniform. Thanks a lot both of you for your help.

Hi Luis,

I try this method and worked for me very well. (sorry for the metric units).

1. Revolve.

2.Sketch base on your drawing. The sketch was made on a plan (on the fly) tangent to the revolve.

I

3.Surface Sweep using the sketch and and the dimensions of the cross section.

Tip. Cap the ends of the sweep.

4.I use Toroidal Bend feature to generate the path. The toridal bend is made on 360 degrees.

5.Solidify with material remove to generate the new surface.

6.I added rounds at the end

I upload the 3D model. Link

Please let me know if you have questions and I'll be glad to help.

Bogdan

Luis,

For the second model is a quick and easy way to do it. (same, sorry for the metric units)

1. Revolve

2. I use Shell for the inside. You can make it in the same feature with revolve.

3. I did a hole on the cylindrical surface and as Offset References I pick two planes, in this case TOP and SIDE. For the Top I put 0 (zero) degrees angel and form the Side the dimension from your drawing.

4. The last step I did a pattern by dimension of the hole.

a. Direction 1 select the Angle and the distance of the hole.

b. Direction 1 Select again the Angle

Final model.

If you include the thickness in the revolve you can have this model done in two features.

Here is the 3D model.

Please let me know if you have any questions and I'll be happy to help.

Take care!

Bogdan