SOLVESPACE -- parametric 2d/3d CAD

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Mirroring groups (extrudes) (by Eloy)
Hi, I'm trying to build a symmetric 3D model, and would like obviously to reuse a half of the design to build automatically the other half. The model will be perfectly symmetric on one plane.

Translate or rotate don't really help me here. How can I mirror groups?
Thu Apr 16 2015, 05:39:17
(no subject) (by yugami)
This may be a bit hacky.

1 sketch the left side, close the sketch so it can be extruded.
2 Extrude
3 Define new workplane 180 from the first
4 go back to g002 and copy the 1st sketch
5 past in new workplane

then re constrain and join together.
Thu Apr 16 2015, 09:07:25
(no subject) (by Eloy)
I've tried that but that seems to loose all constraint information. I'd like to be able to later modify the original group, and have the changes reflected on the mirrored group automatically.

If this is not possible, I guess I can design half of it, and then mirror with other software as a last step...
Thu Apr 16 2015, 10:58:39
(no subject) (by Jonathan Westhues)
Rotate through 180 degrees about the line of symmetry, out of plane and then back into plane. That's still a bit of a hack, but it keeps the parametric link, and doesn't require new constraints.
Thu Apr 16 2015, 13:03:23, download attachment mirrored.slvs
(no subject) (by Eloy)
Thank you for the suggestion. I played with the model you attached, and it doesn't work well when the rotation angle is not 180 degrees. The sketch is properly mirrored, but the extrude is in the direction of the original sketch normal, which is not the actual normal for the mirrored section.

I tried also rotating with copy, 1 time, angle different not 180 degrees. This allows me to extrude each part independently. However, the rotated copy (sketch correctly mirrored) is assigned to the same plane as the original, so the extrude direction is not what I need. I haven't found a way of changing the plane of the rotated copy, or of extruding in the sketch normal :(.

See attached file for example.
Thu Apr 16 2015, 16:41:06, download attachment mirrored_as_copy.slvs
(no subject) (by Jonathan Westhues)
Are you trying to mirror a plane sketch within the plane of that sketch, or something else?

For the plane sketch, the example that I gave is exactly equivalent to mirroring, but the out-of-plane angle must always be exactly 180 degrees. You can mirror about any axis in the sketch plane.

For anything else (e.g., a solid model), that doesn't work. You could draw half in one .slvs file, and then import that into a different .slvs file twice, once with scale of 1, and once with scale of -1.

Or, if you're mirroring a plane sketch, but the mirror image isn't supposed to be coplanar with the original (which I think is what you're doing?), then you could define a new workplane to set the extrusion direction. I've attached an example.
Thu Apr 16 2015, 17:09:48, download attachment mirrored_as_copy-2.slvs
(no subject) (by Eloy)
Hi, sorry for not being clear. I meant that the whole model (multiple sketches/extrudes) will be symmetric with respect to one plane, but each part's sketch and their mirror won't be coplanar necessarily.

Both solutions you propose would be enough, importing with +/-1 scale would be the easiest in my case.

The second would be more work, but it'd have the advantage of seeing both halves before the last step.

However, I don't know how to change the workplane of the rotated sketch. When I try to do it, Solvespace says that the rotated group is in mode 'drawing/constraining in 3d', not in a plane... Could you please point me to some foolproof indications on how to do this?

And a question out of curiosity: is implementing mirroring more complex than repeat? Intuitively, it looks to me as nearly the same operation as repeat rotate.
Thu Apr 16 2015, 18:08:25
(no subject) (by Jonathan Westhues)
The rotation doesn't create a new workplane; I had to do that explicitly. So in the rotation group, I clicked Sketch -> Workplane, clicked a point on the sketch, and constrained the workplane's normal same-orientation with respect to the normal of the rotated circle. I then selected that workplane with Sketch -> In Workplane, and extruded as usual.

And there's nothing specially hard about mirroring; the feature just isn't implemented except upon import.
Thu Apr 16 2015, 18:36:29
(no subject) (by Eloy)
Hi Jonathan,

Thank you for the explanation, finally got it working! I gotta say that this is the first time I run into a problem, for the simple things I do. Usually SolveSpace modelling approach is very intuitive, really good piece of software!
Fri Apr 17 2015, 17:07:14
Retrospective constraint modification? (by Charles Bradshaw)
I am an absolute beginner with solvespace, but have years of experience with parametric 3d modeling.

I draw a simple 2d sketch and constrain with it some dimensions, then extrude it. The elements, lines etc. sketch is still visible and selectable, but the dimensions are no longer visible or selectable .

How do I modify a dimensional or other constraint after the extrude?

Surely "parametric" means the ability to retrospectively modify parameters when one discovers design changes? I hope this is just a newbe question as solvespace is otherwise a brilliant tool.
Wed Mar 7 2018, 09:24:09
Re: Retrospective constraint modification? (by Eric Buijs)
You need to make the sketch that you want to change active in the Property Browser (the floating window in the top-left). To do that click on 'home' and a list of sketches and extrudes becomes visible. Click on the appropriate radio button to make a sketch active. The sketch becomes available again and changes can be made.
Thu Mar 8 2018, 05:47:28
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