Stuck with a variable + derived part

alexander_potochkin

Hello

I have bumped into one problem which puzzles me a lot.
https://cad.onshape.com/documents/497294dde6d7430daccb07c4/w/35ba91b8cf2c45b49165a3a1/e/fba4be4331de47d78cf99bfd

I have a cube and a connector, I use the latter one to create a slot on the cube's side.
It works really well, however when I change the cube's size by changing the #size variable the extrude command fails.

The plain which dissects the cube and the connector is still in place, and I expect the "Use (Project/Convert)" command
to resolve the changed connector's outline.

Any hints how to make it right are really appreciated!

Thanks a lot

andrew_troup

I assumed @joris_kofman  was suggesting an extruded surface, not a revolved one.
That would mean you would could simply pick the end curve of that surface to provide the geometry for your extrude remove profile.

Or even more directly, as I suggested above, use that surface to split the part.

You would not need to derive a silhouette edge for the intersection curve (what you are calling "dissecting" the connecter)
which is the part of your procedure which is failing,
Not entirely surprising, because silhouette edges do tend to lack robustness to model changes

joris_kofman

actually I was thinking that you could create a flat surface of the cross section, with no thickness, and then use the extrude command (through all), but I can absolutely not figure out how to do that.

So I came up with this one in stead. I think this gives the geometry that @alexander_potochkin is actually looking for, if not you can remove the last feature and reverse the cut direction and scope it to everything but the connector.

https://cad.onshape.com/documents/9cba5f3bcb5d49e08debb4d2/w/2b951e15748e48a5be1a3b1d/e/6cd881edd0f64c48a14ff19f

lana

@alexander_potochkin
In Sketch3 notice that vertices are not constrained ( drawn in blue). Before changing variable constrain them to be coincident (dragging out and back in would snap)  then on variable change sketch would regenerate correctly. 

alexander_potochkin

@lana

For some reasons those dots got unconstrained when I changed the cube's size.
(for me this looks like a bug)

Now there are no more lines or dots in blue, but it doesn't solve the problem.
If I change the #size variable the extrude command fails.

For example if you try to change it to 75 the extrude command fails.

joris_kofman

I can see why you are puzzeled. It does not make sense to me either. I think you should contact support and let them have a look at it.

At #size=50 everything looks right, although I don't understand what sketch 2 or plane 1 are for. If I take them out of the equation it still does not work right.
One workaround is to only derive the sketch that you need, since it does not look like you are using the actual body. But ofcourse the workaround does not solve the actual problem

alexander_potochkin

@joris_kofman

Thank you for looking at it, now I know that I am not missing anything obvious :-)

I derived the connector part from another tab and put it at the cube's side with a connector,
I don't think that a derived sketch would work there.
 
To extrude the connector I dissect it with the plane1 and have its outline on sketch3,
sketch2 is just a helper to illustrate the centre of the cube's side.

I'll contact the onshape support, thanks  a lot!

alexander_potochkin

Request #8459 has been filed

andrew_troup

alexander_potochkin said:

..

I derived the connector part from another tab and put it at the cube's side with a connector,
I don't think that a derived sketch would work there.
....

@alexander_potochkin

It seems to be a problem (bug?) for Onshape identifying the silhouette edge of the derived, revolved shape after a rebuild.
You should definitely submit to support.

I did get a derived sketch to work, and it seems to handle resizing the cube OK
 
Here's the edited model:
https://cad.onshape.com/documents/4ae4ab8745e14857aefa5837/w/daa59de5d43a41b28399da47/e/553a5762fe9c4918826131c0

The key was to switch the outline of the left half of your revolve sketch which in your model looked like this :



 from construction to solid, taking advantage of  Onshape's ability to work with any selected portion of the total encosed area of a sketch. 
(I had to edit the revolve, and  reselect just the area shown shaded above)

alexander_potochkin

@andrew_troup 

It is nice to see that you made it work for a derived sketch. 

If only I could position it as I did for the connector part using the mate connectors.

Anyway, I am waiting for the feedback from the onShape team.
I'll keep you posted.

Have a nice weekend!

andrew_troup

@alexander_potochkinThere is at a workaround to transform a sketch (pending Onshape providing the real thing) but the one I'm aware of is laborious :

Basically (to rotate selected entities in a sketch) it involves doing a Circular Pattern, dragging to cue Onshape that you want an "open" pattern (ie not a complete circle) and specifying the desired angle, and a total of two instances including the seed sketch, which is then changed to construction geometry. 

The other is the same idea, with a linear pattern, to translate entities.

An example of the rotate method is given in the "Powerful Workarounds" thread

joris_kofman

you could also create a surface from sketch 1 in connector studio and derive that surface. You could then transform that surface together with the solid and use that as the basis for the cut extrude

andrew_troup

joris_kofman 
Good point. Better still, if a surface was extruded far enough, it could simply be used drectly, to split the part.

alexander_potochkin

@joris_kofman

Hello

I tried to convert the connector to a surface (hitting surface in the revolve command)
and then I derived the service to the cube's studio.

Unfortunately it still doesn't survive a few size changes.
The sketch that dissects the connector to get the extrude template gets broken.
Some dots on it become undefined for no clear reasons.

andrew_troup

I assumed @joris_kofman  was suggesting an extruded surface, not a revolved one.
That would mean you would could simply pick the end curve of that surface to provide the geometry for your extrude remove profile.

Or even more directly, as I suggested above, use that surface to split the part.

You would not need to derive a silhouette edge for the intersection curve (what you are calling "dissecting" the connecter)
which is the part of your procedure which is failing,
Not entirely surprising, because silhouette edges do tend to lack robustness to model changes

joris_kofman

actually I was thinking that you could create a flat surface of the cross section, with no thickness, and then use the extrude command (through all), but I can absolutely not figure out how to do that.

So I came up with this one in stead. I think this gives the geometry that @alexander_potochkin is actually looking for, if not you can remove the last feature and reverse the cut direction and scope it to everything but the connector.

https://cad.onshape.com/documents/9cba5f3bcb5d49e08debb4d2/w/2b951e15748e48a5be1a3b1d/e/6cd881edd0f64c48a14ff19f

alexander_potochkin

Hello

The support answered to my request and offered a workaround similar to what @joris_kofman and @andrew_troup suggested.

Quote:

"Using the silhouette edge conversion is not as stable as we would like to see it. I just split the body and used the face for the profile. See here in this branch of your document:

https://cad.onshape.com/documents/497294dde6d7430daccb07c4/w/6933293970794981a4821d75/e/fba4be4331de47d78cf99b
"

Splitting the part works well and I can go forward with my design now.
However I do hope that the onshape team improve the edge conversion soon.

Thanks everyone!