5 Attachment(s)
So, results for
1. Uncorrected 2. Limited 0.333 3. Limited 0.5 4. Limited 0.667 5. Corrected Attachment 6420Attachment 6421Attachment 6422Attachment 6423Attachment 6424 !!! Stair type of the plot is used to distinguish iteration values better, not the numerical behavior !!! |
2 Attachment(s)
Another issue that I found:
I plotted the pressure residuals for my pimpleFoam solution (see Fig). Attachment 6543 schemes are gradSchemes: cellLimited leastSquares 1; div: upwind laplacian and surface gradients: Gauss linear limited 0.5; limited 0.5; Initial under-relaxation parameters: Code:
p 0.3; I fought with it varying under-relaxation parameters, increasing the step number of the corrections (outer-, neighbor- and non-orthogonality) ; changed the used schemes to fully corrected and removed cell limiting; reduced Courant number to < 1.... Nothing from those helped! Sudden solution was to REMOVE THE UNDER-RELAXATION OF THE MOMENTUM EQUATION ! Attachment 6544 Why is it so, I have now explanation! The whole advantage of the under-relaxation is vanished! For the clarification, final working settings, which removed residuals jump are: Code:
relaxationFactors a) As I understood, in FLUENT relaxation is applied only for the fields (please correct me if I am wrong!). Here in OF's PIMPLE as well as in PISO and SIMPLE algorithms, it is "field under-relaxation" being applied for the pressure versus "matrix under-relaxation" for the momentum equation to increase its diagonal dominance. In presented case according to my observations momentum under-relaxation makes no sense.... b) Is there any way to get initial residuals not solving the linear system in OF? As far as I know, Solver Performance Class returns required information regarding residuals only by means of the "solve" method... Setting maxIter parameter to 0 for the linear solver does not help! BTW, Franco, thanks a lot for indicating this solver parameter, it is rather useful!))) Regards to all... And may the Source be with you!))) Alexander |
Hi All,
I am also trying to do flow simulation for a city model. And using Simplefoam form the same. I am also facing similer kind of issues as MALLALENA please rever to following post for case details. http://http://www.cfd-online.com/For...urbulence.html I was thinking it is due to inlet conditions but I found out that the pressure solwing is getting blown up after few iterations. I am using tetrahedral mesh. Thanks a lot for ur kind help |
Hi All,
I am also trying to do flow simulation for a city model. And using Simplefoam form the same. I am also facing similer kind of issues as MALLALENA please rever to following post for case details. http://http://www.cfd-online.com/For...urbulence.html I was thinking it is due to inlet conditions but I found out that the pressure solwing is getting blown up after few iterations. I am using tetrahedral mesh. Thanks a lot for ur kind help |
Quote:
Similar situation is happening for me. The solution blows up after some time steps. I also have bonding values for K and epsilon. Can you please tell me what did you do to make solution stable. I have also reduced relaxation factor an reltol (0.05) but still not working. Please let me know... |
Hello,
what does this mean? Quote:
Otherwise, you may have bad cells (what checkmesh says?) or schemes which are not good, thus you have to play a bit with them. In any case:
mad |
Hi Maddalena,
My apologies for inconvinience. Can you please help me a bit. I think you have already figured out the way for stable solution. my case details are posted here. http://www.cfd-online.com/Forums/ope...urbulence.html I have also attached check mesh log in the same thread. Thanks a lot for ypur help VJ |
3 Attachment(s)
This is an old topic, but I think it is still of interest to many, so I'll post my findings on the subject here. I had some trouble getting a buoyantPimpleFoam test case to converge, but in the end, I think I managed to get it to converge nicely. I will first describe the case in detail, and then outline the steps I took to improve convergence and accuracy.
I was simulating a simple case of pipe flow in a circular pipe with mesh of just 80000 cells. The solver used here is buoyantPimpleFoam. The flowing fluid is water, initially at temperature of 10 C. I used the icoPoly8 thermodynamics package, with coefficients obtained by fitting a curve to thermophysical property data from NIST webbook. Diameter of the pipe is 140 mm and its length is 1070 mm. The flow velocity at inlet is 0.5 m/s in the positive x-axis direction. The flow is turbulent (Re 10600), and the turbulence model used was the standard k-epsilon. The boundary conditions were set followingly: U: Code:
Inlet: fixed velocity at 0.5 m/s Code:
Inlet: buoyantPressure Code:
Inlet: fixed 283 K Attached you will find my fvSolution and fvSchemes files, as well as a plot of initial residuals vs. time. I made some changes during runTime to these files, which can be seen in the plot. First I played around a bit with the underrelaxation coefficients, but unfortunately I didn't document what I did exactly.
In conlusion, at least for the case in question we found out that:
|
Quote:
Thanks for sharing your findings, keep posting. It's interesting to see how other solvers behave in regards of convergence. |
Quote:
|
All times are GMT -4. The time now is 03:14. |