Solvespace: Is extruding a linked sketch broken?

[vespakoen]

System information

SolveSpace version: edge

Operating system: macOS

Expected behavior

I am trying to replicate the ex-case example from over here: https://solvespace.com/examples.pl
But I somehow cannot re-create it, I wonder if this functionality got removed, if I am doing something wrong, or if this is a bug?

Actual behavior

I cannot extrude a linked sketch

Additional information

I created a sketch, saved it (the sketch layer was active and shown)
Created a new sketch, linked the other sketch and try to extude it, It complains that I need a active workplane first.
I am probably missing some important step here...

[vespakoen]

Just found out that that ex-case example's linked sketch has an activeWorkplane (in the .slvs file) which I don't seem to get when linking something, browsing around the source code to see what's up now.

[vespakoen]

Ok, figured out how to do it, basically importing the other drawing, then selecting "Sketch in Workplane" before doing the Extrude, that all makes sense looking at it now, the error even clearly states what to do.

I feel stupid now... =)

[phkahler]

I had that problem recently. I don't like the extra step needed. It might be a regression but I dont know.

[ruevs]

Ok, figured out how to do it, basically importing the other drawing, then selecting "Sketch in Workplane" before doing the Extrude, that all makes sense looking at it now, the error even clearly states what to do.

I had that problem recently. I don't like the extra step needed. It might be a regression but I dont know.

To me it makes sense - most imported objects are (presumably) 3D ones that are used for assemblies. Thus SolveSpace defaults to Sketch | Anywhere in 3d.

When a sketch is imported it also defaults to Anywhere in 3d and this seems perfectly logical to me - while the sketch was made in a workplane in its original file, when imported it is the "whole" imported file - not just a sketch in a workplane. Thus one needs to select a wokplane (or even create a new one in the same group) and then extrude.

By the way this allows the slanted extrusions that I described here:
https://github.com/solvespace/solvespace/issues/453#issuecomment-642508274
https://github.com/solvespace/solvespace/issues/453#issuecomment-642574190
https://github.com/solvespace/solvespace/issues/628#issuecomment-641756301
https://github.com/solvespace/solvespace/issues/628#issuecomment-641768927
https://github.com/solvespace/solvespace/issues/777#issuecomment-716222105

This is the (updated by @phkahler) reference manual section on this feature:
https://github.com/solvespace/solvespace-web/blob/5627e2628756280ee8a12f43e2d05a3307b1a18b/ref.pl#L1316

Here is one more such example for future readers.
ImportedSketchSlantedExtrusion.zip

P.S. Version 2.0, which is the oldest version I have now, does the same.

[vespakoen]

Yes, it also makes sense to me now, I guess (for the far future) there could be a check if the imported thing is a 2d sketch and then assign it to the correct workplane already or something like that.

Anyways, the error message was clear enough, I guess I just ignored it or something.

Here is the example of what I mean when extruding a linked "Step rotated" thingy.

issue-step-rotated-linked-extruded.zip

[ruevs]

Your problem is that when files are linked in, all entities from all of their active groups are present as geometry. This is documented here https://github.com/solvespace/solvespace-web/blob/5627e2628756280ee8a12f43e2d05a3307b1a18b/ref.pl#L299

In step-rotated.slvs g002 is active and thus the "П" shaped non-closed contour is part of g003 in issue-open-me.slvs. Therefore it does not form a solid when extruded.

If you uncheck g002 in step-rotated.slvs then the extrude immediately becomes a solid.

[vespakoen]

Thanks again for explaining this.

I just tried to do the same with your updated 8040 drawing.
I removed the extrude and hid the sketch.
Now trying to extrude it in another sketch it doesn't work.

I guess this is because it uses 2 step rotates / groups to complete the drawing.

[ruevs]

It works. Leave only g004 (the second rotate group) enabled - it is the only group with a closed contour. See here https://github.com/solvespace/solvespace/issues/841#issuecomment-742518861