Maximum Solver Limitations

[Anonymous]

So the last few days I've been starting at a MacOS beach ball more often than not. 

It seems part of my issue was my sketch had too many points which caused the solver to become overloaded.

In this case, the sketch was a single polygon with 160 edges. I've noticed in other cases, for example, some .svg files where there are hundreds of points. The solver again will struggle. 

Another example. When trying to Fillet many edges. If I select say 50 edges to fillet and change to a fillet size that is not acceptable for one of the edges everything comes to a grinding halt. 

Now in my eyes, I feel like these requests are not that "intense" in the grand scheme of computing power but really what do I know. And I feel like my designs are only gonna get more complicated as my skill progress. Obviously learning to work efficient and smart in both a time and computer solver based approach is part of this progress. 

But clearly beyond my poor design approach. I've overestimated the computer's ability.

My questions after that long winded opener are:

-When it comes to sketches, what are some maximum amount of lines and points you would use before splitting up the sketch?

-What are some bad design intents that would cause solver slowdowns? 

-Does upgrading the CPU allow you to work with bigger and more point dense sketches?

[TheCADWhisperer]

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@Anonymous wrote:

1. In this case, the sketch was a single polygon with 160 edges. 

My questions after that long winded opener are:

2. When it comes to sketches, what are some maximum amount of lines and points you would use before splitting up the sketch?

3. What are some bad design intents that would cause solver slowdowns? 

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1. Attach file here.

2. 7-10 (yep - you read that right)

3. Pattern bodies rather than features.  Pattern features rather than sketch elements. Keep sketches simple.  When in doubt -File>Export and then Attach *.f3d file here.

4. Don’t use someone else’s imported stl rubbish unless your intent is to kill your design.

[jeff_strater · Accepted solution]

My experience does not match with @TheCADWhisperer.  Your questions do not have a simple answer.  It highly depends on what you put into your sketch that is the limiting factor, rather than a simple absolute number of entities.  I've created sketches which have many lines, arcs, etc.

The experience you will have will depend on a variety of factors:

• the number and type of entities in your sketch.  Lines and arcs are pretty efficient, even in large numbers.  Splines (both fit point splines and CV splines), conics, ellipses are more expensive to compute.  Especially fit point splines with a large number of fit points can be slow to compute within the sketch
• the number and type of constraints and dimensions in your sketch.  All constraints are not created equal.  Linear, diameter and radius dimensions, parallel, perpendicular, vertical/horizontal, coincident, colinear geometric constraints are all pretty efficient.  Sketch patterns are very slow, and should be used sparingly (low number of entities, low pattern counts).  Mirror (Symmetry) can also be slow with large number of entities, or complexity of geometry being patterned.  Offset is also expensive, and will affect performance if there are many offsets, or if the offsets are of complex geometry.  The rest of the constraints are somewhat in-between.  Tangent, equal, etc are efficient in relatively small numbers, but if you have lots of tangent constraints in your sketch, it will affect performance

The sketch environment is really intended for interactive creation of surface and solid models.  The usual method is to create geometry for each feature of the design as you go.  If you do that, in most cases, each sketch will be fairly simple.  Where things can fall apart is if you try to put too much into one sketch, or try to implement things like fillets in the sketch, rather than in the solid environment (each fillet has two tangent constraints).  Similarly, do your patterning/mirroring in the solid environment instead of the sketch.  Use more sketches rather than fewer large sketches.  Use the "fix/unfix" trick to isolate parts of a larger sketch that is "finished".

I will say that sketch performance is an area that we want to focus on going forward, so hopefully things will improve over time.

Hope this is helpful.

[Anonymous]

Really, well I'm glad I asked the question because I was always under the thought that work should be done in sketches and not solids. Filleting a solid vs in a sketch just seems wrong but in the end, it does make sense. Most of the time when I'm designing something it is never a finished product. I often link sketch dimensions so I can make quick and easy changes. In the case of making life easier for the solver.

Is it best to link sketch dimensions or use individual dimensions?

Sometimes I use dimensions from some of the very early sketch and link them to new dimensions on downstream sketches. Should linked dimensions really just be used inside single sketches. 

[TheCADWhisperer]

Canyou Attach an example file here?