Cadding Ridges on a Cam

[Thad House]

We are trying to add ridges to our tensioning cams, similar to the WCP cams. How do you actually add the ridges to the curve in inventor? I cannot figure any way at all to do this. Any advice?

[inventor_phild]

Not completely clear on what is required, but I am assuming you need a pattern of grooves around the cam surface.

1. Create a new sketch on the face of the cam. The outside edge shoul dbe projected.

2. Sketch the profile of the groove.

3. Extrude > Cut the profile.

4. Circular pattern to create the remaining grooves. You may have to play with the groove dimensions to get a correct solution.

Tip: Try using construction lines from the center to define the groove width e.g. 5 degrees apart.

If this does not work or make sense, send me the part and I will try it.

[Thad House]

So I am trying to CAD the outer profile of this
http://www.wcproducts.net/217-3431/
Making the main outer shape is easy, because it is just a polar equation. Making the ridges along that outer shape wasn't working for me. Using a circular pattern required a constant radius from what I could tell, while the piece does not have a constant radius.

[inventor_phild]

OK, got it now.

1. Assuming you have the cam profile already modeled.

2. Create a sketch on the front face.

3. Sketch the ridge profile at the start of the cam profile.

3. Extrude > Cut the profile.

4. Now comes the little known feature of Rectangular Pattern. Using Rectangular Pattern, select the extruded feature.

5. For Direction 1, select the sketch profile of the cam. You may have to make a visible sketch for this.

6. Enter the number of ridges.

7. At the bottom left of the dialog box, select Curve Length from the list.

8. Click OK.

Again, if you cannot get his to work, email me the part file with the ridge sketch created and I will create the pattern.