Cutting a pocket in a curve

dylan_lynch

I can't figure out how to get a sketch tangent to a curve.

For a simple case: If I want to cut a hole in the side of a cylinder, how would I go about that using a sketch? Is it possible to do this without a Boolean or is that the way to go? Auxillary question: If that is the way to go how can I move the second part in the Part Studio (or copy the arrangement from an assembly back to the Part studio)?

lougallo

@dylan_lynch This would be easier when we have a split face tool.  Steps to do it now:"

1. For now we create a plane outside the part
2. Extrude up to surface of the part with the profile (as NEW)
3. Use Thicken-> Remove to cut the face back the desired depth,  (select touching face of toolbody

brucebartlett

I think Boolean would be the way to go? 

1 Extrude your tool against the cylinder face
2 Move tool
3 Boolean Subtract

Alternatively you could also create a surface on the cylinder face thicken then Boolean. this would get the pocket faces normal to the cylinder face. 

Take screen shot and upload, a picture will tell us more.

dylan_lynch

Ok, played with it more and made some progress. I made the circular hole using a sketch drawn on the Front plane there. This works for through-all stuff.

For the pocket on the side there I had to create the plane through the center of the cylinder and then make the second plane using an offset. Then I could draw a sketch and make a pocket.

I guess my question now is: How do I create that plane directly (if at all). Is there a way to draw a plane tangent to a curve? Edit: to clarify: Offset works well when you have a cylinder but if I have a more complicated curved surface it seems to become a lot more difficult.

lougallo

@dylan_lynch This would be easier when we have a split face tool.  Steps to do it now:"

1. For now we create a plane outside the part
2. Extrude up to surface of the part with the profile (as NEW)
3. Use Thicken-> Remove to cut the face back the desired depth,  (select touching face of toolbody

brucebartlett

I'd also done a simlar thing with a 3 point plane extruding up to curved surface from behind. "Thicken" with the Remove works a treat.
@LouGallo yes split face would be great here so you don't end up with a tool.

brucebartlett

dylan_lynch

That's a neat trick! Thanks for the help  

øyvind_kaurstad

When this question was asked and answered, it wasn't possible to split faces, so one had to extrude a tool to do it, like @lougallo showed in the accepted answer.

However, now that we can split faces, it is possible to avoid the toolbody by using the sketh to directly split the target face. However, this poses a new problem that I don't see how to deal with: If the target body has a continuous face (like a cylinder has), then the split face command will split the face also on the far side of the cylinder. You can of course then use the thicken cut on just one of the split faces, but if I then want to use a circular face pattern to copy this hole/pocket, it will fail if one of the copies overlaps the far side split face.

This document illustrates the issue:

https://cad.onshape.com/documents/06e0c5e59725061543294565/w/96b80c914ff3d0cca1d48ea2

In the part studio called "toolbody", I used the method outlined by @lougallo, and then patterned the hole. In the part studio "split face" I tried to do the same using the split face command, but the pattern fails since one of the copies exactly overlaps the splitted face on the far side. If the pattern count is 3 or 5 it works, since no copy will then overlap exactly.

I'm not sure if this is the correct behaviour? This is of course easy enough to work around (either just use the old method, or pre-split the target surface so that the final split isn't replicated on the far side), but shouldn't this have worked without doing such tricks?

jakeramsley

øyvind_kaurstad said:

I'm not sure if this is the correct behaviour? This is of course easy enough to work around (either just use the old method, or pre-split the target surface so that the final split isn't replicated on the far side), but shouldn't this have worked without doing such tricks?

The behavior is correct in my view because you are telling it to copy and rotate faces around the part and one of them is going to fail because it is trying to create a duplicate face.

In the meantime, a really simple solution is to delete that extra face before patterning.  Since the cylinder is analytic, it will correctly close the cylinder back into a single face and allow the pattern to succeed.

øyvind_kaurstad

@jakeramsley Boy do I feel stupid now. I did think of that, but when right-clicking on the face to delete, there is no option to delete the face. You have to use the 'Delete Face' toolbar command to make it work.

Ah well, no harm done, and learned something along the way. Thanks.  :-)