Helix Split Test

_Ðave_

 I had presumed that if I were to manage to split a part it would be two separate pieces. Therefore in my public document " Helix Split Test " I've accomplished splitting a tube with a helical extrusion by using Boolean-Remove but the resultant parts are still one part. It appears that my presumption is incorrect. Can anyone clarify for me or suggest a method to accomplish splitting this tube on a helix and removing one half.

Thanks All

shanshan

DaVicki , I think there is a misunderstanding about "split a part", when you use "boolean-subtract" for splitting the part in your document, actually it can  not been splitted by this helix shape(part 2),the remaining part is a single part,it did not be divided into two parts.there is also another tool for splitting a part,namely "split",but here you also can not split the part by this"split"tool.

Narayan_K

@ DaVicki  , To make them two piece you have to cut in twp place.If you cut in one place it will be cutting a circular cylinder to make it flat.

_Ðave_

@shanshan Thanks, What was I thinking!! Yes, of course it is still one piece.

Dave

andrew_troup

@DaVicki This is a really counterintuitive situation, and I had to try to "fix" your model before I realised it.

It's not an Onshape issue, it's an issue with topology. What you have modelled is actually a single body, and you could roll it flat. 

It's like the core of a roll of toilet paper, or a strangely proportioned spring (regardless of how many turns it has, a spring is a single body)

_Ðave_

andrew_troup said:

@DaVicki This is a really counterintuitive situation,
 

I would phrased it a bit differently but I like  counterintuitive situation much better.

Thanks, Dave

andrew_troup

OK, Here's my study model - I edited it by lengthening the profile line for the sweep so it created another helical split surface opposite the first (by reasoning that a "two start" thread had two separate grooves, so a "two start spring" must have two separate bodies.) As soon as I did that, the "Split" feature started to work.

https://cad.onshape.com/documents/b44e56afe96b418d8ff9b836/w/e2dc917921604b38b4930a00/e/a66ef772d5a64413bdd5fded

I copied @DaVicki's  lead in thickening a surface to produce the hollow cylinder, but normally I would do a solid extrude of two concentric circles.

I didn't do a Boolean subtract; I used "Split (Part)" because I figured that was what Dave was setting out to try to achieve.

Here's the helical SURFACE (not solid body) I used as the tool for the  Split (Part) Feature :

(the straight line is the path: the helix is not used, except to make a coincident constraint for one end of the 
profile line. I made the profile as two lines, equal length and parallel, but I could have used a midpoint constraint of one line to the path, probably. It was just a quick and dirty adaptation of the previous model, which was the same but "single start" and if failed to split the body, for topological rather than capability reasons, as mentioned earlier.)



So here's a thought experiment which might convince those who still think Dave's original was two bodies: if you laser-fuse one of the helical interfaces between the two bodies in my solid model in this post, you effectively end up with what he tried to model, but your weld has combined them into one body.

_Ðave_

@andrew_troup Thanks for outlining this, very helpful.

matthew_menard

I think unrolling a cardboard toilet paper roll or similar will yield a nearly identical single piece as @DaVicki 's original model.  I thought it should be two pieces at first as well.