Does anyone know if there is a way to cr …
Does anyone know if there is a way to create a wrap on the surface of a cylinder that meets up with it self to create a continuous debossd groove? The attached picture shows one of the cylinders that I am trying to create with a pin track on its surface. In this picture I used the wrap function to deboss the track sketch onto the surface of the cylinder and then created a circular pattern with 6 instances of the deboss. If you look at the picture there are small discontinuities in the track that are created because solidworks doesn’t seem to like having circular patterns or single wraps intersecting. 
JeffM 8:42 am on May 13, 2009 Permalink
It’s a matter of doing the math correctly. Wrap is probably the best way to go. Create a construction line that is equal to the circumference of the cylinder, then create your sketch.
One thing I recall, was that you sometimes have to fudge where the sketch starts, though I don’t remember the specifics.
sttcraig 9:34 am on May 13, 2009 Permalink
JeffM
Thank you for your comment. When I make the sketch exactly 1/6 of the circumference of the cylinder, I get the following error.
Feature CirPattern1 failed to rebuild, which may cause subsequent features to fail. Would you like to repair CirPattern1 before SolidWorks rebuilds the subsequent features?
This is because the pattern would intersect at the start and finish of each repetition of the sketch (which is what I want). In the screen capture, I made the sketch a little less than 1/6 the circumference so this error doesn’t occur, but I end up with the gaps you see in the cylinder track.
superpilun 10:16 am on May 13, 2009 Permalink
The problem probably has something to do with zero thickness. SolidWorks doesn’t like functions that try to do this sort of thing. Fortunately there is a pretty easy work around. Create only one wrap feature. Then cut a 1/6 pie slice out of the cylinder where the wrap feature is. Then use a circular pattern on the BODY. Then use the Combine feature to merge them all together.
sttcraig 11:44 am on May 13, 2009 Permalink
superpilun,
Is this what you were getting at (see screen shot)? If I line up the extrude 60 degree cut with the wrap feature I get an error so I had to offset it a bit. With this wedge, it creates the circular pattern, but the wrap no longer shows up. Also the combined feature is greyed out so it can’t be used….probably because of the root problem
CBL 1:01 pm on May 13, 2009 Permalink
No need to combine bodies. Just pattern the feature, but make sure the feature is slightly more than 1/6th, and select the Geometry Pattern option.
sttcraig 2:18 pm on May 13, 2009 Permalink
Okay, I am getting there but there still seems to be an issue. I wrapped the feature, then did an extruded cut of 1/6th of the cylinder, and then tried to use the circular pattern feature. It shows exactly what I want in the yellow outline, but won’t actually do the circular pattern.
sttcraig 2:22 pm on May 13, 2009 Permalink
superpilun 2:51 pm on May 13, 2009 Permalink
craig, I have problem viewing any screengrabs you may have posted because of internet restrictions at my company. e-mail me at pchen (@) bankspower.com and I can help you with your model (seems like a very simple issue)
admin 3:01 pm on May 13, 2009 Permalink
Could you upload the model to the post so we can give it a try?
sttcraig 3:30 pm on May 13, 2009 Permalink
I finally figured out how to get this to work. I need to tinker a little more to get it perfect, but here is what I did to solve the problem.
I had to select the first cylindrical extrude, the wrap feature,and the second pie shaped (1/6 circumference) as features to pattern, plus have the geometry pattern option selected.
Thank you for all the help on this.
Sean
JeffM 7:42 am on May 15, 2009 Permalink
Another way to do it is to create a linear pattern in a 2d sketch and then wrap it around the cylinder.