Cannot split curved part with curved surface

martin_danger

Hi, 
https://cad.onshape.com/documents/30aa714d9ba1405b6c4962b3/w/abd3881b0b7f5b4bdc438106/e/422cc167d73e7cdd700f89e3
I'm getting an error when trying to split my circular part. 
I've extruded a surface from a line that I sketched using the spline tool. 
At first, I thought the error was from the surface starting/ending at exactly that same place as the part but extending the surface past the part boundary didn't help. 
The error is unhelpful - it says I should check the input. 

Can anyone spot what Onshape is unhappy about with my inputs? 

p.s. how do I resize images that I insert into the post? These are huge...

S1mon

I’m pretty sure you need to split the ring into two parts. You can’t make a zero thickness split like that. You could make a very thin cut if you want a split ring.

wayne_sauder

The easiest way I've found to do things like this.

https://cad.onshape.com/documents/3cf276f8301baff7a0db7759/w/1e158608d1e9ff9271528a0b/e/b2531bfb2e5e72f82fd36e6c
 

rafael_telgmann

Hi, if the ring have to be a part with a split, the split must have thickness.
https://cad.onshape.com/documents/80bf22684ee4190d6b5e8707/w/97687269d77daaf87ac5c29e/e/25e3164a0d723fa2ba82eafa?renderMode=0&tangentEdgeStyle=1&uiState=669540989a078755030dc31c

Resizing images is still a mystery to me too. but it is possible...on this thread the gifs were huge, now they are as intended.
https://forum.onshape.com/discussion/24026/forum-images-messed-up

GregBrown

A couple of things:
1. You cannot create non-manifold geometry in Onshape - the geometry engine will disallow it. Therefore you cannot split the wheel with a single surface (as this zero thickness cut would attempt to create non-manifold geometry)
2. The axis of the circular pattern you used is not the axis of the wheel...

Knowing this, have a look at my document. I created a Mate connector to be the axis of the circular pattern. I Boolean merged two of the three surfaces and used them to split the part. I then split the part one final time with the remaining surface.

(The three surfaces could not be boolean merged into one as that would, yes... create non-manifold geometry.

The initial surfaces (I assigned appearances for clarity):


After the boolean merge:


After the two split features (I did not "keep tools"):

https://cad.onshape.com/documents/7ceab33ba94460b718f1a013/w/13174314ff0975a7688fb585/e/17c2c37e71b6be252d9483d3

[Edited to add: the last Part studio in my doc ^^^ has a crazy but effective way to achieve it using only one split feature... ]

robert_scott_jr_

A similar 'problem' was the subject of a somewhat recent post and the (now obvious) explanation made me chuckle. A split must result in more than one part. - Scotty

Split:

verb

1. break or cause to break forcibly into parts, especially into halves

martin_danger

Thanks for all your comments and suggestions. I did realise the split issue (that a split must result in 2 parts) later but then the ideas I came up with to get around this all hit brick walls - see https://forum.onshape.com/discussion/24582/how-to-split-a-circular-part-my-journey-so-far#latest
The options here are very helpful - it's great to have a forum like this to help with ideas when I run out of new ideas myself.

martin_danger

robert_scott_jr_ said:

A similar 'problem' was the subject of a somewhat recent post and the (now obvious) explanation made me chuckle. A split must result in more than one part. - Scotty

Split:

verb

1. break or cause to break forcibly into parts, especially into halves

Yes, that particular definition is the one this tool most closely resembles and in retrospect, it's obvious. However, before I knew the answer, "split" to me could mean other things. For instance, if you split your skin, you still only have one continuous layer of skin, albeit with a, lets call it a local discontinuity.