How to cut a section on an oblique plane in an assembly tab?

OpenR2

I defined a plane that I want to use for section cuts in a part studio.
How can I use this plane in the assembly studio as reference for the section cut?
My workaround was to slice my reference cylinder so there was hard geometry to use as reference but this was a very roundabout solution.
What am I missing?

NeilCooke

If you create a sketch on the plane you can insert the sketch into the assembly and use the face of the sketch to create your section. 

viru

@OpenR2, You can use mate connector as reference plane which will be created on origin. Kindly refer below video for more detail.

Specific to your issue:- You can create mate connector at same plane position which you used for section cuts in a part studio. This mate connector automatically reflect in assembly studio. Now you can select mate connector as a section plane and you can get desired section. Kindly refer below video

lougallo

In addition to Mate connectors, you can now also move (snap) the section triad to place it in the correct position as well.

OpenR2

Lou/Viru ..... there is no physical geometry in the model that would infer the plane. Only construction geometry. So how would I use that construction plane as the basis for the assembly studio section?

NeilCooke

If you create a sketch on the plane you can insert the sketch into the assembly and use the face of the sketch to create your section. 

OpenR2

Neil,

This pointed me in the right direction.

But this is the perfect example of how things that appear to be simple in OnShape are actually harder compared to other CAD systems.
The functionality to use Sketches for section definition in Assembly studio is there but its only 80%.
Here's why I say that.... 

When inserting the sketch into the assembly the icon that allows sketches to show up in the list has to be in the activated state. You have to know to click the sketch filter button. The sketch filter is set to filter the sketches by default.

Once the sketch is inserted into the assembly there seems to be some gotchas on the section dialog.

You can't pick the sketch from the tree .... this seem silly because there is only one support plane for a sketch and that should be the plane used for the section.

You can't pick just any element on the sketch. Hovering over a point or a line doesn't highlight the sketch. Only hovering over the closed volume of a sketch lets the sketch be selected. In my case the sketch just had the point and the line that I needed to orient the instance.

In order for the sketch to work...I had to fake in some geometry to make a closed area.

The ability to put sketches in an assembly was not something I was aware of. Thats my bad. I either missed that from the start or missed the update that introduced the functionality.

From OnShapes side....not being able to pick the sketch from the tree, not being able to pick the sketch from any geometry in the sketch, and force the user to create an unnecessary closed area....this seems like its not quite done. Not really 100% thought out. An 80% solution.

But with some extra (unnecessary) geometry ... you got me up and running.

Thank you.

NeilCooke

@OpenR2

I'm glad you're up and running.    

Using a skech as a section plane is a workaround. Sections require faces, and sketches comprise faces and edges so that's why you must pick the sketch face. 

Onshape works differently in many ways to other CAD systems, but unfortunately every CAD system has workarounds to cater for everybody's needs. 

Being less than a year old we don't have every feature and function of 20 year old CAD systems, but we're working on it. 

Thank you for your continued support and the offer still stands if you need any help.