My simulation model has 5.4 million cell, so solver runs very slow. I can't wait it to be coverged. I just stop it running. It is in 225 steps out of total 429. The monitored mass flow rate has been balanced among BC openings. I attached one screen shot here. I'd appreciate if somebody here has comments regarding the result converged or not.
Thank you in advance.
Thank you, Bill. This is my first CFD analysis using FS with structure mesh cell. I agree that more unstructured mesh nodes could catch more domain features, especially in boundary layer, more inflation layers can predict pressure loss quite accurately. When I switch to SWFS, tutorials mention that more cells can make result more accurate if solver converged well. I don't doubt this as well. I just set up this model as level 5 with automatic refinements. The cell # comes with 5.4 million. With those # my machine still can run, even though slow. This is a test for my machine limit as well.
I just want to know, based on your experience, if result above image showing could be thought converged already even though it is not converged from FS software. There is little variations for those parameters going though till the end.
hard to tell from the way you have it presented. I usually plot only like quantites and use the absolute scales and then adjustting them to get the sort of resolution one needs to make a good call on it. I would run it at level 3 with thin wall optimization on and nother else. If you have a small gap somewhere - use a local mesh control. Thre are a couple papers from Mentor Graphics on the b'layer handling and the decretization scheme the upshot of which are that you do not need to worry about the mesh in the b'layer - the program handles it with the wall model and the wall model is formulated to cover all situations. On the descretization it just shows you how the scheme compares to unstructured and structured schemes - which is very favorable in terms of convergence - ie it is very close to hex structured convergence yet can handle arbitrary geometries with ease.
Thank you, Bill. After this, i will try level 3 with min.gap of 0.1" in fluid region.
I would not use that min gap number as it will be a global setting and drive very high cell counts. use a local mesh control to ensure you get 4 or 5 cells across the gap.
something else to note, there is no guarantee that the problem will converge in 1 travel either. so while you're 250/429, it might actually take 1.5-2 travels to completely converge.
the only real way to know if you can stop it is if the results are near what you expect.
bring the problem down to a reasonable number of cells, see what the answer is, go up some more, see what the answer is...etc. this should be the same for any analysis tool. start simple, start coarse. did you approach it differently in other software?
something from my experience, i was working with a customer that wanted a very high cell count because of experience with other tools. i they had around 10million cells. i solved the same problem on my system in a fraction of the time with 10000 cells, and the answer was within about 1% of expected. 10million cells gave a bit more definition to some of the plots, but the values of importance for this customer were acheivble with far less cells.
Hi, Bill and Jared,
I reduced the cell numbers and run two scenarios. The results posted here. First one has only 35760 cells with level 3 & inserted local mesh on the curved edges. The 2nd one's cell increased to 196,730 with level 3 & inserted local mesh on the curved edges, plus turn min. gap size on automatically. Both have been converged as per mass flow rate criteria.
The results comparison as the following: from which, It looks like more cells, more accurate result (close to test data). That's teh reason I would like to use more mesh if I could.
Thanks for comments.
hannah, just to make sure i'm clear, you're comparing results that are completely converged to results that are partially converged? (lower cell count vs higher cell count)
a swing from 74/100 to 248 i don't think will come from mesh alone. this probably needs a bit more investigation.
For above 3 scenarios, physical model hasn't been touched. BC keep the same. Only mesh setting was changed as the above menstioned.
The solver with two lower cell count converged as shown, with warning message. I doubt the result is right as well in these two. Butthe case with higher cell count shows result close to we expect even though it hasn't being converged totally.
In this case, I feel more comforable using more cells than less cell #. I have no solidworks FS experience. Hopefully I could get it up since now.
I am trying an arrangement to make a comparison between Ansys CFX and SWFS.
consider that during convergence of your high cell count problem, it may go down to the 100/74 value. if that happens, which answer is correct?
the only way to know which one is right is by understanding what the answer is likely to be based on your experience of the system or physical testing. comparing software vs software isn't a good way to validate a solution. what if you make the same incorrect assumptions between them?
if it were me, i'd really be looking at more than just the goals to understand how the problems are different.
Thank you, Jared. I have to leave this topic as it is now. But I will come back after 2 weeks from my vaction and hope you enjoy your summer.
hannah
sounds good. might be worth leaving your computer on running that 5million cell problem to see if it converges! been there, done that. and if i'm curious, i use logmein to take a look at the solution from my iphone
Thanks for suggestion. I will leave it to run. But I wont't bother myself to think a bit it during holidays.
Jared, I got your email already. I will discuss with my boss regarding the training. And let you know later.
Thanks
Regard
why would you need so many cells? You say need 5 across a gap to get a decent velocity profile....It would probably help top remember that flow sim uses the cut cell approximation for he geometry and hence has structured hex dominated mesh. It is not like unstructured codes where you need a large amount of elements to get a decent number and they take a large number if iterations to converge. Assuming you have covered that one off then there is a large set of tools to lower cell counts from mesh controls to component modeling techniques. The last model you posted looked, in my estiamte to be able to be done with under 100,000 cells and still get a good answer but it is hard to know from looking at an image.