Computational Cost of Different Constraints

[Anonymous]

I like to do my sketches with LOTS of parameters, construction lines, and constraints, and for the most part, it works well.  However, as the sketches get more complex, things get much laggier to edit, and I'll randomly start to get "compute failed" when it worked previously and I've changed literally nothing about the sketch. 

While I'm sure that this already awesome program will continue to get better and more robust with time, in the mean time it might be helpful to know which constraints are more computationally expensive or likely to lead to errors (if such things are known).  There's often more than one way to do something, and it would be good to know which way is typically more optimal.

To give an example of the sort of problem I'm trying to solve, I'd like to know, if I have a short line segment that will lie entirely on a construction line, would it be better to:

A. Set the segment as collinear with the line?

B. Set the segment as parallel and one endpoint as coincident with the line?

C. Set both endpoints of the segment as coincident with the line?

Or will it really not make a difference?  I'd be surprised if there were no difference, because it really SEEMS like collinear takes longer for fusion to compute than the other options.

Any tips, observations, or even suspicions would be welcome.  Thanks! 🙂

[TrippyLighting]

Can you share an example of such a sketch ?

[Anonymous]

Below is part of one. 

Please understand: there's no particular drawing I'm asking for help with.  I'm trying to find out, in general, what constraints are harder for fusion to calculate and what ones are easier.  In the case below, I learned, that fusion really doesn't like it when I sketch half of something symmetrical and just mirror it.  However, among the other constraints, it's harder for me to be certain which are preferable, but I still imagine the computational costs add up.

[TrippyLighting · Accepted solution]

1. The mirror and equal constraints are the worst offenders and should be avoided. In your sketch they easily can and should be completely avoided by mirroring the solid not the sketch.
2. Pattern constraints can be very computationally heavy. Particularly as you've mirrored patterned objects. If you want to keep the features to be patterned in this sketch, that's fine. However, make an extrusion of the base shape without the cut-outs. Then extrude-cut these in a second step and pattern the feature.
3. Filleting also is better left to solid features than done in a sketch.

[innovatenate · Accepted solution]

I've found Tangent Constraints can be challenging as well (in addition to pattern and mirror constraints). Often there are two solutions with tangent constraints, for example a point on a circle that are 180 degrees from each other where the solver will get "confused." It's not always avoidable, but @TrippyLighting has a pretty good suggestion to minimize by using a 3D fillet command when you can. 

If you run across any egregious, reproducible examples where the constraint solver is struggling, please share them over in the Support board. We are happy to report these to development to help drive improvements.

[Anonymous]

Very good tips.  I like the idea of doing more work with a solid rather than leaving it all in the sketch.

I just want to make sure I understand your suggestion regarding the pattern.  It sounds like I should: extrude the overall shape, extrude out a single instance of the hole shape to cut it, then pattern the hole feature.  Did I get that right?

It sounds like this is hinting at another tip I didn't realize.  Is it computationally easier for Fusion to do the main extrusion and then the cut rather than doing the extrusion with the hole to begin with?

Thanks again for the tips.  I also hadn't realized that about equals, so I'll make a point of steering clear there as well.

[TrippyLighting]

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hunter.rayner wrote:

I just want to make sure I understand your suggestion regarding the pattern.  It sounds like I should: extrude the overall shape, extrude out a single instance of the hole shape to cut it, then pattern the hole feature.  Did I get that right?

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Yep Exactly!

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@Anonymous wrote:

 Is it computationally easier for Fusion to do the main extrusion and then the cut rather than doing the extrusion with the hole to begin with?

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Yes, that is also the case by an order of magnitude. There are a good number of honeycomb threads that demonstrate the difference quite effectively 😉