Static Stress Simulation slow with Local Solve

[henry.harvey]

Hi,

When I do a static stress simulation locally it is very slow but it does not appear to be using any significant system resources (everything is below 10%, CPU, GPU, RAM...) 

I can understand a complex simulation being slow but my computer doesn't seem to be doing much!

PC specs:

AMD Ryzen 7 1700 8 core 3Ghz

16GB 3200Mhz RAM

GTX1060 6GB

Thanks

[mcmillr]

Hi Henry, is it possible the file save is taking a long time? We always save your file before starting a local solve.

To test this, make a change to your file that will cause it to require another solve (suppress/unsuppress a load) and click Save, then press ok when prompted for the version description. Now pay close attention to the version number to the right of your file name on the tab at the top of your document window. This will eventually increment to the next higher number when the save is complete. Now do your local solve. If it is much faster then the save time is your issue.

If it isn't the file save, can you describe what you are seeing when the solve is running? You can expand the line in the Job status dialog and it will show you what step is being performed and provide a progress bar for each step. If the Job status dialog doesn't even display for a long while, then this also indicates the time is being spent uploading the file to create a new version.

[henry.harvey]

Hi Rob,

Thanks for the reply. I followed your instructions regarding saving the file. I didn't make a difference to the solve time. I expanded the Job Status dialog. "Preparing Model" and Generating Contacts" was almost instant. Meshing status bar took several minutes to become fully blue but then stayed there for about 5 minutes before it actually said "Complete". See attachment. The PC was basically idling all this time. The final status bar "Solving" I think, took a few minutes but did cause the PC to bump up to about 50% CPU and 50% RAM.

Thanks

[mcmillr]

Thanks Henry, the picture makes it clear.

Your CPUs are 11% busy, which isn't idling, it just means that only about 1 core is being utilized. (100% / 8 cores = 12.5%)

Meshing can leverage multiple cores if you have several parts, and the solve will leverage multiple cores, but not all the time.

If your model took several minutes to mesh, it isn't small, and there is probably some time spent toward the end of meshing which is single threaded, plus we also need to write the mesh data to disk, and this can also take a bit of time. We will use very little CPU when writing/reading files. The mesh is written to a folder under %TEMP% which is usually on your C drive, so if this disk is pretty full or fragmented I suppose this could be making IO slower than usual.

Also, if you are forcing the mesher to generate small elements it might be slowing things down more than needed. We use 'high order tetrahedrons' for the mesh and this does not require a small mesh size to get accurate results usually. You can run with the default of 10% of model size, and if you want increased accuracy, turn on adaptive mesh refinement (if the Study type supports it) and this will refine the mesh only where needed. You can also use 'local mesh refinement' to refine specific areas without using a small mesh everywhere.

The only other thing I could do would be to run your model myself and make sure there isn't anything unexpected going on.

[henry.harvey]

Hi Rob,

I agree it was an exaggeration to say idle, but it was often sitting at 5% CPU use during this process. My new SSD has plenty of free space and R/W(Max) 3,200MB/s/1500MB/s so that shouldn't be an issue. I think I found the TEMP folder you mentioned - does appear to be on my SSD. I've attached a screenshot of my mesh settings, I think they are all at default. I've also attached the file, it would be very interesting for me if you could run the simulation on your machine. 

Thanks

[mcmillr]

OK I see the problem. This is a progress bar 'bug', plus your model is a bit difficult to mesh as-is.

We have several meshing 'phases' and sometimes the 'solid' meshing phase fails and we need to refine the surface triangles, then try to calculate the solid mesh again. This is especially common on parts that are thin and/or have some very small faces relative to the overall model size. Our progress meter apparently is reporting 100% even though the solid mesh phase failed and we need to go back and do *several* more passes. I will log a defect as I can see why this could lead you to believe something is not working correctly.

Also, our mesher can only use 1 CPU per part, so your system will at most be 12.5% busy the entire time we are meshing. If you look at FEACSCommandLine.exe and mg-tetra.exe you will see them using 100% of a single CPU.

If you want your model to mesh in 20 seconds (give or take), do this:

Go to the Model env and drag the last sketch, extrude, and mirror feature so they occur BEFORE the fillets. Then move your end of timeline marker before the first fillet. These fillets are 'cosmetic' and should not have a large impact on your Sim results.

Now switch to Sim and see how fast you mesh and solve!

We also have a Simplify environment with tools to remove fillets, but these tools work directly with the geometry and can't always remove fillets 'after the fact'. If you have modeled the part in Fusion, you can get better results by suppressing the fillets in the model. I realize this isn't ideal, but hopefully it will allow you to get the job done.

[henry.harvey]

Thanks for trying out the model - everything you have said makes sense to me except the removal of fillets. I'm not a mechanical engineer but I was under the impression that even small fillets can hugely improve the strength of injection molded parts by spreading forces and preventing point stresses on corners and edges.

However I did two solves for comparison - one with fillets suppressed as you suggested and one with fillets. To my surprise the filleted version received a much lower Safety Factor score

and showed critical stress right on a fillet where previously there had been a sharp internal corner and no issues! Please see attachment.

[mcmillr]

Henry, I discussed this with one of our solver developers and we have some recommendations:

1) The fillets may increase strength slightly in reality, but they also greatly increase geometric complexity, they make your iterations take a lot longer, and they might result in a false stress concentration or singularity.

2) Removing the fillets should not impact accuracy that much PROVIDED your mesh size is dense enough to capture actual min SF/max Stress.

Using the 'no fillet' version, set your Average element size to 5%, and set Adaptive Mesh Refinement to High. This will produce a nicely converged Von Mises stress value, at a safety factor of ~1.2. 

I also get a decently fast result just setting the avg. mesh element size to 1% and disabling adaptive refinement. For a thin part like this, a small global mesh size may be warranted, although you could also try doing face splits around the areas you are getting high stress and applying a local mesh refinement to these areas only and keeping the mesh coarse everywhere else.

Sorry I don't have one 'easy' answer, but hopefully this gives you some options to play with.

[to3dornottobe]

I am experiencing the same lag of performance. A simple 20x20 steel tube, 1.5mm wall thickness, R2 edges takes 25 minutes to solve locally. most of the time the CPU load is 1,5-2%. CPU is a 10th gen I7, 32gb ram. It used to be quicker with more complex aluminium profiles. What's going on? Saving the file to a new version is a matter of 2 seconds.

[TheCADWhisperer]

@to3dornottobe 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?