Generate sketch from part

fma

Hi,

Is there a way to generate a sketch from a part, by defining a custom cut or projection plane?

bruce_williams

The 'Intersection' command does this.  It is under the 'Use' command icon.  Choose part(s) and the intersection of part(s) and sketch plane is created.

Another way to make relational sketch entities is to use the 'Offset' command.  It is not necessary to first convert with the 'Use' command when the goal is offset curves. 

mahir

It's hokey, but a work around for that is to split the part with the sketch plane, use an intersect within a sketch on the resulting cut surface, then use a boolean to reunite the separate bodies.

https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/c3b358533cdb341de5650652

shanshan

there is a "Use" command in sketch , you can generate sketch from any part with it 

fma

Thanks. But it does not work exactly as I expect; I would like to get the intersection between the part and the sketch plane...

bruce_williams

The 'Intersection' command does this.  It is under the 'Use' command icon.  Choose part(s) and the intersection of part(s) and sketch plane is created.

Another way to make relational sketch entities is to use the 'Offset' command.  It is not necessary to first convert with the 'Use' command when the goal is offset curves. 

fma

The intersection tool is for faces, not parts. You have to select all faces! For external ones, it is OK, but for internal ones, this is very complicated.
More, if you change the sketch plane, all is gone.

In fact, the Section View is close to what I'm looking for, but I didn't find a way to generate the sketch of the intersection... Is it possible? If not, it would be great to implement it (and not too difficult, I think)...

mahir

It's hokey, but a work around for that is to split the part with the sketch plane, use an intersect within a sketch on the resulting cut surface, then use a boolean to reunite the separate bodies.

https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/c3b358533cdb341de5650652

fma

Thanks for the work around! It works fine.

Is it possible to make such operations automatically using FeatureScript? I didn't dig yet into this powerfull feature...

mahir

There are various ways to section parts in FeatureScript, but there is no FS equivalent of the Use and Intersect functions. So you can't really automate the creation of a sketch using those functions.

lana

Copy part , split copy, use split face in sketch, delete both pieces of copy  would give you a better downstream performance than merging pieces back together. 

mahir

What @lana said. I was trying to automate that same procedure with FS when I ran into the Use/Intersect limitation.

fma

Ok, I see.