Need help modeling a cam slot around and through the edge of a cylinder.

john_lopez363

I have a need to create a cylindrical part that has a cam slot radially and laterally around it's radius.   For the life of me I cannot figure out how to model it.

The cam slot start and end needs to be precisely placed at 90 degrees apart radially and 10mm apart laterally.  The pic is  an example of something similar... it is the cam slot feature that I'm trying to create.

Any help would be greatly appreciated.

Thanks

bryan_lagrange

See if this helps. All I did was wrap a slot on a tube with the ends 90 degrees apart. 

https://cad.onshape.com/documents/7c39a800ad820e05972b17d8/w/6a565141c724d9e6ec53d59d/e/9425ec311cee6ae308713639

glen_dewsbury

@john_lopez363
Here's one way to do this.
I treated it as sheet metal to make cam sketch easy.
Sketch 1 angle leave open at 5deg or more to make finish easier.
#dev variable is measured long edge in flat view.
Draw cam sketch in flat view.
90deg = #dev/4
Finish sheet metal part and close with replace face.
Go back to sketch 1 and change the angle to .002deg to make error irrelevant. #dev will update on its own.
https://cad.onshape.com/documents/4ca0229f69e5013bbd25e104/w/0721279ba72bb0e922174b8e/e/3819b509d930ca8de663cea3

Guess I forgot to hit post. This has been sitting for a while, LOL

bryan_lagrange

See if this helps. All I did was wrap a slot on a tube with the ends 90 degrees apart. 

https://cad.onshape.com/documents/7c39a800ad820e05972b17d8/w/6a565141c724d9e6ec53d59d/e/9425ec311cee6ae308713639

glen_dewsbury

@john_lopez363
Here's one way to do this.
I treated it as sheet metal to make cam sketch easy.
Sketch 1 angle leave open at 5deg or more to make finish easier.
#dev variable is measured long edge in flat view.
Draw cam sketch in flat view.
90deg = #dev/4
Finish sheet metal part and close with replace face.
Go back to sketch 1 and change the angle to .002deg to make error irrelevant. #dev will update on its own.
https://cad.onshape.com/documents/4ca0229f69e5013bbd25e104/w/0721279ba72bb0e922174b8e/e/3819b509d930ca8de663cea3

Guess I forgot to hit post. This has been sitting for a while, LOL

bryan_lagrange

In part 2 I have the center to center dimension 10mm apart.

glen_dewsbury

@bryan_lagrange
@john_lopez363
Just playing now. Wanted to see if could make it all the way around. 
https://cad.onshape.com/documents/4ca0229f69e5013bbd25e104/w/0721279ba72bb0e922174b8e/e/08323533a54d1584422ada2c

bryan_lagrange

@glen_dewsbury  nice. Check out my part 3 in the Onshape doc I posted.

glen_dewsbury

@bryan_lagrange
Never thought of wrap continuing past 360 deg.

john_lopez363

@bryan_lagrange @glen_dewsbury... thanks guys, both solutions obviously work.  Between me posting the original ask for help and me seeing these responses I did figure out yet another way.

I added a Helix around the cylinder at 1/4 turn and 10mm height, Swept a Surface using the Helix curve as the sweep path and then Thickened (remove) the surface and added some end features to finish up.
 https://cad.onshape.com/documents/a4b5d329e8109d54a8f3517e/w/042e7c4a6850105343fb1662/e/1eeeaac9298f0210290cc3d9

While all of these "solutions" obviously work, to be honest they kinda feel like hacks.  It would be nice if OnShape enhanced either the Slot Tool so that it could follow a Helix or 3D Spline OR added a new tool to do the same. Perhaps combining some aspects from the Hole Tool and some from the Sweep tool together with the sweep path following 3D curves or splines.

bryan_lagrange

@john_lopez363 I don't know if I would call it a hack. If I were to create this in Solid Edge I would utilize a similar technique. I don't deal with a lot of work like this since I primarily work in sheet metal, so there could be an easier way of doing this. Onshape is still fairly new and does not YET contain all the features you currently have in a mature software such as in Solid Edge and solidworks. With new functionality being posted every 3 weeks eventually we will see these features currently not present. If you create an improvement request, I am sure those who have to create geometry like this would jump on board and help push it along in the development roadmap.

Having feature script allows users to create functionality that is not currently present in the software. I am sure if you ask the community, one of the feature script gurus could probably create something.

One thing I will give the Onshape team is that they are not quick to release something just to say the software has it. They do a good job of testing it and in most cases  improve on what is currently there in the market before releasing it to ensure it functions properly.

Just my 2 cents.

glen_dewsbury

@john_lopez363
@bryan_lagrange
Hey John. Bryan's method gets my vote. Doesn't get any cleaner.
When I see the delete parts feature it makes me suspicious of the surfaces in your slot. I suspect that out of parallel and such that could cause the cam to bind or be loose. The nature of the surface you made combined with the thicken as well as straight extrudes does not line up if you look closely. The wrap brings an accurate surface then thickens normal to the surface giving a much better result.
Note that I did not use radius' in my sample, but conics instead for a better acceleration in and out of linear sections.
https://cad.onshape.com/documents/1a9a224235cd8b597d25d1d0/w/cabb1926d5d9b8d2b41ab900/e/648b98b2feb6a50be552062f