lofting from a sketch gets screwed up by other sketches on the same plane

stuart_robinson

this feels like a bug because the Loft menu box says "Face of Sketch 1" but it's showing a bunch of shapes that are distinctly *not* in "Sketch 1"

to avoid lots of zooming and clicking, do i have to put all these sketches on their own planes?  

eric_pesty

Can you expand the "face of sketch1" selection the loft, I wonder if you somehow ended up with the face of the solid in there as well...

_anton

The problem (or at least one of them) is that loft doesn't support faces with inner loops (mouse over the red feature dialog header), and the red shapes are those loops.

stuart_robinson

@eric_pesty when i tried that earlier it didn't seem to show anything useful. just said "Face of Sketch 1" again i think

eric_pesty

@_anton
He's saying he only selected sketch1 which doesn't have any internal regions. But the red preview does suggest there is a face of the solid selected in there somehow.

You also only have one selection for the loft, did you try picking another profile for the loft to see if it solves it? It could just be a graphical glitch (refreshing should also clear that if that's the case).

We might be able to figure what's going on if you share a link to your doc...
 

stuart_robinson

ok i think i figured out what's happening.  example here

when you create a "New sketch" from the surface of a Part, this new sketch becomes cursed forever by the ghost of the Part's perimeter in that plane

i'm worried that this is a Feature since i could imagine it could be useful at times if someone is aware of the behavior, but it's caused headaches for me before, and seems distinctly bad.  since i feel like you should be able to see that something is a Sketch, and understand everything about the Sketch from the Sketch itself.  without needing to remember hidden artifacts lingering around as side effects from the specific way that Sketch happened to be created.

for example, here i have two sketches.  Sketch 1 is clearly a circle, and Sketch 2 is clearly a rectangle



now i'd like to loft my rectangle:


but i cant.  because there's an undead circle hiding inside it that i cant get rid of,

because of how the rectangle was created. (by creating a "New sketch" from the other end of an extrusion of the circle sketch)





https://cad.onshape.com/documents/a82f03eed8bf29ae67e2de8e/w/2e833e275c987e44d42fc3d0/e/d854c39f0f00246eaa8f19d4

stuart_robinson

so actually now that i understand how this works, i've been able to use it to solve a lot of other problems and it's really powerful and useful.  but i do still think it's a bad design.  unintuitive/cryptic 

eric_pesty

stuart_robinson said:

so actually now that i understand how this works, i've been able to use it to solve a lot of other problems and it's really powerful and useful.  but i do still think it's a bad design.  unintuitive/cryptic 

You can also turn it off in the sketch dialogue using the "disable imprinting" checkbox...

stuart_robinson

oh wow TIL "imprinting", thank you @eric_pesty!

nick_papageorge073

Disable imprinting should be clicked on by default. My very strong opinion:) I've purposely wanted it maybe 2 times in 3 years. Every single other time I have to click that checkbox. And when my co-workers don't click that box, it becomes a mess.

glen_dewsbury

nick_papageorge073 said:

Disable imprinting should be clicked on by default. My very strong opinion:) I've purposely wanted it maybe 2 times in 3 years. Every single other time I have to click that checkbox. And when my co-workers don't click that box, it becomes a mess.

Cast a vote here.
https://forum.onshape.com/discussion/comment/101644#Comment_101644