SOLVESPACE -- parametric 2d/3d CAD

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Add non repeated features to repeated pattern (by Paul)
I'm making templates for motor laminations. Motors are made from stacks of thin slices to reduce eddy currents. Anyway, I've make a single stator tooth and can use step-rotating to create the full stator. The angular width and number of teeth can easily be changed (see attachment). One question is: Is the resultant shape a single piece? It seems to be. The main question is: How do I add features to it after the step-rotate? I need to add a few bosses around the outside to both it together and hold end caps on. Can these be added and become part of the same work piece without human intervention (after I change tooth geometry)?? A similar problem will exist for putting a keyway in the rotor laminations by the shaft.

What's the best way to add these features?

Also, is there anything I could be doing better here?

Tue Apr 7 2015, 20:25:38, download attachment stator.slvs
(no subject) (by Jonathan Westhues)
As attached? You could just sketch the features, extrude them, and Boolean union them onto the solid model. You can then export with File -> Export 2d Section.
Tue Apr 7 2015, 21:04:13, download attachment
(no subject) (by yugami)
You can either add them prior to the extrude; a circle drawn on the surface will act like a delete. Or you can define a new work plane and draw them on that, then extrude and select deference instead of union and pull the extrude into the stator.

In your case since the holes need to be on every lamination I would do the former.
Tue Apr 7 2015, 21:04:36, download attachment stator (1).slvs
(no subject) (by yugami)
I was assuming you needed holes like in the motors I've taken apart.
Tue Apr 7 2015, 21:05:17
(no subject) (by Paul)
Neither is quite what I wanted. But first, Jonathans file shows a smooth outline when I open it and looks like what I want. But when I click on other groups and then back to the last group it no longer looks like that - its separate pieces. This seems like a bug - why would it appear different just because I looked away for a minute?

I like the yugami approach too, but the holes are really supposed to be outside the outer ring. Of course hobby motors it may not matter. BTW I mistyped "bolt" the end caps on.

Neither of these solutions works if I go back to the first group and change the overall radius. I'm hoping to be able to make different motors by just changing dimensions and not have to manipulate geometry. Completely parametric.

I could have bosses on the outside that would move automatically with radius if the stator was a circle and not a replicated section.

BTW getting this right is just a bonus to me. SolveSpace is the first OSS CAD I've found where I can actually do this kind of thing at all. Impressive work Jonathan!
Tue Apr 7 2015, 22:48:47
(no subject) (by Jonathan Westhues)
When you select another group, the lines and curves from that group (in addition to the edges of the solid model) get shown. To return to the model as initially viewed, choose "hide all" in the browser.

And I didn't constrain the additional feature in my example; but you could constrain it with respect to the outer circle if you wanted, and the model would be fully parametric.

Let me know if you have any other questions.
Wed Apr 8 2015, 00:22:09
Possible bug (by Paul)
I tried this again with better results. I left the outer diameter off the first sketch - keeping it to just the stator tooth. Then after step-rotate I built the outer ring with bosses complete with parameters. Two problems came up during this.

1) All things drawn in the second group appear as construction lines by default. I could still toggle them to be real geometry, but the default was different. Is there a reason for this, or is it a bug? I'm using the Mac version.

2) I was unable to change the number of items in the step-rotate after creating the additional geometry. I can still change parameters on the stator-tooth sketch and they change in the second group, but changing the number of them doesn't work. This makes sense to me because anything attached to them after replication would be problematic with entities being removed or added. In my case it was a little annoying because the outer ring is only anchored to the origin and not the previous geometry, but they share a point at the origin. Some simple tests show it doesn't have to interfere with the previously built stuff, but in my case they share that one center point. Is it possible to use "the origin" as a point? I just clicked in the middle which could be the origin or any of the other points that were already there.

I'll attach the new version for grins. You can change parameters but not tooth count.
Sun Apr 12 2015, 20:06:39, download attachment exp1.slvs
(no subject) (by Jonathan Westhues)
(1) That's deliberate; my expectation was that entities in step-and-repeat groups would generally be construction entities used to help constrain the step distance/angle. You can always toggle it back, as you observe.

I didn't generally expect people to put much extra geometry in step-and-repeat groups. Instead, I expect them to extrude the step-and-repeat, and then add more features later with Boolean operations on the solid model. You can do that even if you just want a 2d part, by extruding to some arbitrary constant depth.

(2) If you hide all groups except g001-#references, and then select the point at (0, 0, 0), then you can be sure you have the origin and not some other point that happens to be constrained there.
Mon Apr 13 2015, 03:15:15
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