Scaling breaks sketch
@anthonyrossi01 wrote:I would guess I am missing something about Constraints yet all of the tutorials I have watched don't really apply to lines that touch end to end.
@anthonyrossi01 - doing a bit of reading between the lines here - when you say "My issue is that the drawing breaks when I try to scale it. ", in addition to the missing coincident constraints that @TheCADWhisperer pointed out, I assume that you also mean: "sketch scale removes dimensions in the sketch". (a "drawing" refers to the 2d documentation found in the Drawings workspace). Yes, this is correct. If I start with this:
and then scale it by 2, I get:
All the dimensions have been removed. This is just how Sketch Scale works. It is a brute-force scale operation. It does not attempt to scale by adjusting dimensions (I'm not sure that would even be possible, to be honest). So, to keep the intent of the scale, existing dimensions must be removed.
You can easily design a sketch that can be scaled, using user parameters and equations cleverly, but that is a much harder task. Better off to do your scale, then re-dimension.
Jeff Strater
Engineering Director
We can go through your entire design step-by-step resolving each issue as we go.
Note in Sketch 1 that there are 4 blue circles...
@anthonyrossi01 - @TheCADWhisperer is trying to help. If he is being terse, it's because he responds to 20 or more of these a day, and does not always have time to type out a long response. Some people will know what "white dots" means, others will not.
The design you shared was not marked to allow download, so we can't take a look at the model ourselves.
What @TheCADWhisperer is referring to is: The white dots indicate a lack of coincident constraints between adjacent curves. If such a constraint exists, no dot is drawn at the intersection:
why does this matter? Because, when you move (and scale causes a move) a sketch line, a coincident constraint will ensure that they stay together. In the image below, I've moved the right hand lines upward in both cases:
That may be the source of the issues you are seeing. That's the best guess we can make without seeing the actual design itself.
Jeff Strater
Engineering Director
aha. Having the design reveals a lot. This looks like a bug in sketch scale. I suspect the reason why it fails on this design is that this geometry is not on the sketch plane. It is what Fusion considers "3D" sketch geometry. Some operations are harder on 3D geometry than 2D geometry on the sketch plane. In particular, 3D arcs are difficult, and I suspect what is at the root of this problem.
Since this particular sketch looks like it is inherently 2D, I would keep the geometry on the sketch plane - most things will be easier/more reliable on 2D geometry
The Fusion bug for this is: FUS-76667
Jeff Strater
Engineering Director
if it were me, that sketch is simple enough that I would just re-draw it, at the correct size, and on a sketch plane. That way, you would not have to even scale the thing at all. It would be quick enough to do:
BTW, I did test this, and you can scale it, and the sketch does not come apart, but you do lose the dimensions. Again, that can be avoided by just drawing it the correct size to begin with.
Scaled version:
which, I think, validates my assumption that the problem is the 3D geometry.
Jeff Strater
Engineering Director
"You are saying take the dimensions off the model and recreate the sketch meaning measure angles of straight lines and then create tangents to connect them that way the tangents are never scaled?"
No, sorry, that is not what I meant to imply. The tangent arcs scale just fine if they are 2D (on the sketch plane). The flipping happens only in 3D. I meant only that, instead of creating a sketch that needs to be scaled, just create it at the size you are going for after the scale. Instead of creating a sketch that is 7.5mm and scaling it up by, say 1.5x, just create it at 11.25mm the first time.
Jeff Strater
Engineering Director
