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Cant extrude included file as in reference, why? (by Rune)
Hi, I try to follow the refernce " it is possible to draw a section in file A, import that section into file B ..., and then extrude it ...in file B."

I cannot get it to work. Attached a (a circle) and b (another circle and an import of a.slvs). When I try to extrude g003-a it gives me: "Error... Select a workplane before extruding" but that does not seem to work.

Any explanation is appreciated.
Thanks in advance
Fri Nov 7 2014, 08:41:49, download attachment a.zip
(no subject) (by Jonathan Westhues)
That error message isn't very clear. To extrude the imported plane sketch:

(1) Activate that group in the browser window.
(2) Select a workplane, whose normal will define the extrusion direction, by left-clicking; it will turn red.
(3) Choose Sketch -> In Workplane.
(4) Choose New Group -> Extrude.

Let me know if that works, or if you have any other questions.
Sun Nov 9 2014, 20:11:27
(no subject) (by Rune)
Got it. I never selected the workplane by clicking on it (Point 2). I propose you add your 4 points to the reference manual.
Normally point 3 would give me: "No workplane selected. Activating default workplane" and I have extruded. So the catch is that there is no 'default' workplane for imported files?
BTW. what is a 'default' workplane, I'm a bit confused about the difference between the menus 1.New Group - sketch in new workplane
2. Sketch - sketch in workplane and 3. Sketch - Workplane
I expected the workplane to be automatically selected when I select it in the browser window.

Thank you very much for the explanation.
Mon Nov 10 2014, 03:58:11
(no subject) (by Jonathan Westhues)
"Sketch in New Workplane" groups automatically create a workplane, and that's the default workplane for the group. Other kinds of group don't have a default workplane.

In any kind of group, you can draw and constrain entities either in 3d (Sketch -> Anywhere in 3d) or in a particular workplane (Sketch -> In Workplane). Initially, "Sketch in New Workplane" groups use their default workplane, and other groups are in 3d. You can change that later with those two commands.

You can use any workplane in any group, and you can use multiple workplanes (or a combination of workplanes and entities or constraints in 3d) in a single group. So you might, for example, sketch a line in workplane A, and then constrain its length as projected into workplane B, all within one group. That's an elegant way to express some kinds of geometry, though in most cases too complex to use practically.
Mon Nov 10 2014, 04:49:20
(no subject) (by vicente cavanna)
I encountered a similar issue with my version 3.0~0e0b0252 and thought at first glance that this thread holds the solution to my problem, and it does but with some differences in the process which I will describe here for the benefit of others.

I verified that the given solution works in version 2.3~7c1ca460. The only clarification I would like to make is that step 3 of the given process must be performed even if the menu shows a checkmark next to "sketch in workplane" implying that Solvespace is in "sketch in workplane mode".

In my version however, the given solution does not allow me to specify the workplane!

The only way I have found to specify the workplane is to select the (rectangular) outline of the plane. If I select the workplane thus then the process works.
Sun Aug 29 2021, 17:22:59
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