Failure to compute upon changing a parameter

[robertmarteau]

Hi,

I have a pretty simple design that I'm trying to make parametric.

The idea is to keep the shape/proportions when the exterior diameter changes.

That is why I expressed all dimensions based on d_ext (exterior diameter). 

"d_ext*[value]".

The initial value of d_ext is 380mm. But when I try to change the value (for example set it to 350mm), it fails to solve and shows me almost all (but not all) dimensions relative to that d_ext value in red.

Can someone point me in the right direction to solve this issue ?

Note: please excuse the cutesy writings, this is a birthday gift for my mom... 😉

Thanks in advance for your help,

Stan

[HughesTooling]

My advice is avoid mirroring in a sketch like the plague! The symmetry constraint is a very expensive constraint to solve and if you have more than a few will slow solving and in this case make it fail.

I've removed all symmetry constants and replaced with either horizontal\vertical and equal constraints and added a few coincident constraint to make a fully constrained sketch, note padlock one the sketch in the browser. All skatches should be fully constrained. See attached design.

[HughesTooling · Accepted solution]

Looking at your other sketch with the warning I see you have auto project enable but you have also manually projected edges so you have lines on top of lines.

You also have a rouge midpoint constraint that's causing a conflict.

Easiest way to fix was to delete the construction line then redraw and add a midpoint to the filleted rectangle (best practice would be not to fillet in the sketch and keep it as simple as possible and fillet the solid body.

Here I've fixed the sketch and fully constrained. Note the construction line is now constrained at both ends.

See attached design. you really need to be more careful and fully constrain sketches.

[HughesTooling]

In your first sketch you have an unconstrained line you do not need on top of another line.

If you delete the longer line then add back the angle dimension the sketch shows fully constrained.

@jeff_strater I'm was a bit confused how this sketch is solving as fully constrained until I noticed there are 3 circular patterns! Would be good if these were not stacked.

[jeff_strater]

good point, @HughesTooling - I'll put that in as a bug - you are right, Fusion should not stack sketch constraints like that.

[edit] created bug FUS-146985 for this

[robertmarteau]

Hi,

Thanks so much for your help ! I had absolutely no idea about the "cost" of solving constraint, but it's good to know!

I was convinced I had made a more "fundamental" (or I should maybe say "stupid") mistake than that.

@HughesTooling: your remark about fillets in sketches is duly noted, and - retrospectively - I don't really know why I didn't do that right from the start... It's also way quicker to do than to draw these rounded corners in the sketch, so there's really no reason not to do it...