Sketch: Intersect of a face not working (plane does)

outstanding

The sketch mode Intersect tool mentions that it would be able to:

"Project the intersection of a surface, or face ... to the active sketch plane"

This does not work from a face of a part. 


Steps:

• In sketch mode, select Intersect tool
• select the face as shown in the picture

Expectation:

• I will get a line on the active sketch, presenting the intersection of said face (extension of it) with the sketch plane.

Actual:

• An error banner shows up: 

Work-around:

- Create a plane (before the Sketch step); offset 0mm from the said part face
- Use intersection with said plane; that works

The document to showcase this: https://cad.onshape.com/documents/453d32f9a17ead3e10d896cc/w/a0d1a3cbe0b284d7419b19da/e/b8139646234764853c29e822?renderMode=0&uiState=64abb4efd68a1263fd1ee8c4

// I need this in making veneer constructs, with angles between the plates, to project the neighbouring plane to one, in order to create "teeth" between the parts.

glen_dewsbury

It would appear that in the sketch mode the intersect has to be an actual intersect with the sketch plane and will not project.
You can use projected curve in 3D mode to place a curve on any given face that can be used later to make a sketch.
https://cad.onshape.com/documents/d2668de69711420f803a74b4/w/10bdd4c3ecd73814b8a3dc0d/e/0baf52182dd690c3c53e9a40

outstanding

The reason I posted this was to help Onshape study what seems to me as a conflict of documentation and actual functionality. I'd like the tool to function as intended in the docs (that mention surface or face five times).

NeilCooke

The description is in the name of the tool - intersection. A coincident face has “infinite” intersections. Use “use/project”. 

S1mon

The tool works fine. I've used it tons of times. You shared your doc via link and didn't make it public, so it's not possible to see exactly how you were trying to use it. The sketch plane and the surface need to intersect.

outstanding

S1mon said:

The tool works fine. I've used it tons of times. You shared your doc via link and didn't make it public, so it's not possible to see exactly how you were trying to use it. The sketch plane and the surface need to intersect.

That explains why a Plane would cut it (pun) and a face wouldn't. I thought Onshape could extend the face, i.e. show the intersection of its extension. btw. the document does not mention the two must intersect, so I didn't know...

As to sharing, I thought I've made the document as public as I can. Will try to find out what's the recommended way to share an MVP.

outstanding

NeilCooke said:

The description is in the name of the tool - intersection. A coincident face has “infinite” intersections. Use “use/project”. 

Use would not do what I want, without an interim sketch. The two sections are not in a 90° angle to each other (though this is not very visible in the screenshot) so it matters whether a projection happens orthogonal to the sketch plane (Use does this) or as the extension of the face, on the said sketch.

EvanReese

Assuming the face is always planar, you should be able manually create a line and set it to coincident with the face. This should give you an effect similar to extending the face and intersecting it.

glen_dewsbury

Thanks Evan. Just learned something new.
I did note that the line I drew did not want to have any existing constraints like hor/vert since the coincident causes over constrained condition.

outstanding

@Evan_Reese Thanks: that works!! I had not come to realize that I can constrain with out-of-sketch entities. That is simply brilliant and elegant.

EvanReese

@glen_dewsbury
ah yeah good thought. That could happen. Onshape seems to do pretty well at not failing with redundant constraints, but not always. One of the modifier keys (maybe shift?) disables automatic constraint snapping to make that easier to not add.

@asko_kauppi
I use that one a lot since faces are usually a more stable reference than an edge, especially if it's a pretty big fundamental face.