SOLVESPACE -- parametric 2d/3d CAD

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copy and pasting with constraints? (by Zack)
I just found solvespace and I'm totally flabbergasted by how awesome it is, and how well it's been designed. I've been struggling with FreeCAD, and Creo Elements, and SS just kinda clicked...

Anyhow, I'm using SS to make a case out of laser cut acrylic, so I'm creating each unique layer in the case as a single part. The case will be held together by 3mm bolts going through all the layers, so I've got a lot of circles in the exact same places on each part. Since every layer has the same exterior shape and bolt holes, I tried to create a fully constrained dummy part and then copy paste the part into new parts, but the constraints are lost in the process. This also happens when copy-pasting within a part. I have a lot of hex nut cutouts that I have to reconstrain individually even though the 'parent' hex is only constrained to itself and nothing else.

Is this expected behavior, or I am being particular dense and missing a method for doing this simply and quickly?

Thu Feb 27 2014, 21:07:43, download attachment back_cover.slvs
(no subject) (by Jonathan Westhues)
As you observe, cut and paste works only on entities. There are cases where it would be nice for that to also work on constraints, but I haven't implemented that yet.

In your case, though, it may be preferable to draw the holes and hex cutouts in separate sketches, and then import those sketches into each part that uses them. That keeps the structure parametric. So after drawing the parts, for example, you could make a change to a hole location in one place, and the change would propagate into each part that used the hole pattern when you regenerated it.

To do that, create a file with a single plane sketch, for example the holes. Create a different file for the part, and import (New Group -> Import / Assemble) the plane sketch into the part. Then, place the plane sketch where you want it (for example, with one point-coincident constraint, and one same-orientation constraint).

To extrude the circles to cylindrical cuts, select a workplane parallel to your sketch plane, and choose Sketch -> In Workplane. The sketch will be extruded perpendicular to that workplane. (When you choose New Group -> Sketch in New Workplane, a workplane gets activated automatically. In this case, we need to do it by hand.) Then, choose New Group -> Extrude.

You might also be able to use New Group -> Step and Repeat Translating to your advantage. If you set the number of copies to one, and start "with copy #1", then that makes a copy of the active sketch that you can drag anywhere in the plane. That avoids the need to draw complicated geometry multiple times, and again keeps the parametric link. You can step and repeat a single source sketch multiple times if necessary.

Let me know if you have any trouble. I've attached an example.
Fri Feb 28 2014, 08:02:26, download attachment
Thanks! (by Zack)

Thanks for the quick response... Quite frankly I was baffled by your directions and I was messing around for about 30 min attempting to extrude the imported plane. The problem was that I had "Hide workplanes from inactive groups" option mistakenly enabled, so I couldn't use the existing workplane! Then I just had to remind myself to select the workplane and use the "Sketch -> In Workplane (2)" option. Worked wonderfully after I'd figured that out.

Another question for the hoi polloi: Anyone running this under VirtualBox? I can't get Wine to behave well enough (running Ubuntu 13.10 and Wine 1.7 with the Nouveau graphics drivers), so have resorted to a W7 VM. It got super choppy after creating an assembly with 4 parts, and I'm wondering if anyone has the same issues running it under Vbox. I've got 2GB RAM allocated to the VM, as well as the max video memory (256MB). I can't enable 3d acceleration as it creates all sorts of awful tearing and artifacts in SS.

Sat Mar 1 2014, 17:45:45
(no subject) (by Zack)

I spoke too soon. Looks like seamless mode in virtualbox was the culprit. If I run SS in a windowed VM, it works well with 3d acceleration enabled.

Sat Mar 1 2014, 18:09:36
(no subject) (by Jonathan Westhues)
Note that the workplane just needs to be parallel to the sketch plane; it doesn't necessarily need to contain the sketch. (The workplane defines the extrusion direction, but the offset of the workplane from the origin is ignored.) So you could also have just used one of the coordinate planes, which are visible even when the automatically-generated workplanes from "sketch in new workplane" groups are hidden.

Let me know if you have any other questions.
Sun Mar 2 2014, 18:26:59
(no subject) (by Zack)
Ah, good to know, I could swear I attempted that, but it's entire possible I'd did that before I realized I wasn't then using the "Sketch -> In workplane" option.

Sun Mar 2 2014, 19:16:09
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