
[Sponsors] 
April 5, 2010, 03:46 
simpleFoam convergence on large domain

#1 
New Member
Knut W
Join Date: Apr 2010
Posts: 1
Rep Power: 0 
Hi,
I am having difficulties getting convergence with simpleFoam on a large domain  350 x 300 x 100 meters. Case is air flow around buildings. There are two inlets, one on the side of the box, 300x100m, and one in the centre (a stack) with diameter of 0.6m both with abut 10m/s. After about 40 time steps I start getting "bounding for epsilon" and soon "time step continuity error" runs off to large values, and calculations fail. Mesh is tet from Salome. Looks ok(?), but since domain is big I have difficulties getting cell sizes too small. Average cell length is 2.5m for the domain and 0.3m for a sub mesh around the stack tip. What I have tried without success: * refining mesh (limited by 3GB ram, though) * Lowering relax factors to 0.3 * Increasing epsilon initial value (tried a few settings) * lowered p relTol to 0.01 Any suggestions as to what to try next? Cheers, knut  my system: OF1.5 on caelinux 2009  checkMesh reports: Create time Create polyMesh for time = constant Time = constant Mesh stats points: 251432 faces: 2567968 internal faces: 2406476 cells: 1243611 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 1243611 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Topological cell zipup check OK. Face vertices OK. Faceface connectivity OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface inn 22354 11338 ok (not multiply connected) ut 22354 11338 ok (not multiply connected) veggs 20356 10359 ok (not multiply connected) veggn 20356 10359 ok (not multiply connected) pipe 65 40 ok (not multiply connected) vegg 76007 38531 ok (not multiply connected) Checking geometry... Domain bounding box: (106.777 110.777 0) (290 245.442 100) Boundary openness (1.04978e15 9.99092e15 6.43789e14) OK. Max cell openness = 3.74724e16 OK. Max aspect ratio = 62.5 OK. Minumum face area = 0.0102578. Maximum face area = 28.7368. Face area magnitudes OK. Min volume = 0.000662881. Max volume = 46.6845. Total volume = 1.03156e+07. Cell volumes OK. Mesh nonorthogonality Max: 88.0021 average: 16.1696 *Number of severely nonorthogonal faces: 14. Nonorthogonality check OK. <<Writing 14 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 0.86499 OK. All angles in faces OK. All face flatness OK. Mesh OK. 

April 6, 2010, 10:09 

#2 
New Member
Join Date: Apr 2009
Posts: 26
Rep Power: 9 
I would suggest to run a couple of hundreds of steps without turbulence (set "turbulence" to "off" in constant/RASProperties). Then turn it "on" while the simulation is running.
If it does not initial converge without turbulence generate an initial field from "potentialFoam writep" Ask 

April 15, 2010, 21:31 

#3 
New Member

Hi,
My domain is complex, I generate the mesh with gambit. After performing checkMesh, the results display as follows: Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 137559 faces: 398938 internal faces: 385622 cells: 130760 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 130760 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology wall 12708 12762 ok (nonclosed singly connected) inlet 96 119 ok (nonclosed singly connected) outlet 512 545 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.1 0.15 0.94) (0.0749999 0.0874996 0.4) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (4.04084e19 2.40544e19 1.16605e19) OK. Max cell openness = 3.73953e16 OK. Max aspect ratio = 134.96 OK. Minumum face area = 1.6845e08. Maximum face area = 0.000211397. Face area magnitudes OK. Min volume = 2.10562e10. Max volume = 6.46656e07. Total volume = 0.0135334. Cell volumes OK. Mesh nonorthogonality Max: 81.9702 average: 7.09614 *Number of severely nonorthogonal faces: 36. Nonorthogonality check OK. <<Writing 36 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. ***Max skewness = 7.55797, 12 highly skew faces detected which may impair the quality of the results <<Writing 12 skew faces to set skewFaces Failed 1 mesh checks. End What does "Failed 1 mesh checks." mean? When I use sipmleFoam and ke model with upwind schemes(Divergence schemes), it works well. But after changing upwind to highlevel schemes, it can't get convergence! what should I do to improve it? Thanks! 

April 16, 2010, 02:22 

#4 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
checkMesh is failing because you have highly skewed cells (and also some strongly nonorthogonal cell)
The second problem can probably be corrected indirectly with nonorthogonal correctors in the solver. For the first one, you've to reconsider the mesh. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 22, 2010, 22:27 

#6 
New Member

Hi,
The checkmesh result of my new mesh is as follows. The simplefoam with highlevel schemes Still does not work. Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology wall 6102 6143 ok (nonclosed singly connected) outlet 336 361 ok (nonclosed singly connected) inlet 72 90 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.1 0.207 0.86) (0.1 0.1 0.375) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (3.14905e19 1.76981e20 7.25013e19) OK. Max cell openness = 3.11283e16 OK. Max aspect ratio = 35.1393 OK. Minumum face area = 4.64258e07. Maximum face area = 0.000339005. Face area magnitudes OK. Min volume = 6.96387e09. Max volume = 1.40468e06. Total volume = 0.0216753. Cell volumes OK. Mesh nonorthogonality Max: 81.1011 average: 7.28001 *Number of severely nonorthogonal faces: 18. Nonorthogonality check OK. <<Writing 18 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 1.77958 OK. Mesh OK. End 

April 23, 2010, 00:18 

#7 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Try to see if there is some point in particular in the mesh where the solution is not correct.
Can you post your fvSchemes and fvSolution too?
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 23, 2010, 03:22 

#8 
New Member

Hi,
This is my fvsolution and fvscheme.My turbulent model is RNGkepsilon model. Once I change the scheme of div(phi,k) and div(phi,epsilon) to other high order scheme, it display "floatingpoint error". In addition, similar problems have emerged with the LRR model even if all the schemes are set to upwind like this: div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwid; Thanks beauty 

April 23, 2010, 14:17 

#9 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
You can still use second order schemes, but using limiters, usually without any need to go back to first order schemes.
In your scheme settings, you might have a problem with div(phi,U) Gauss linear corrected; Try running your case with div(phi, U) Gauss linearUpwindV cellLimited Gauss linear 1; which preserves the second order accuracy almost everywhere, preventing instabilties. In addition, you could post the actual error message, so we can see where the problem actually comes from. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 24, 2010, 03:43 
RSM can not get convergence!

#11 
New Member

Hi, Alberto
After changing the schemes as your advice, the simpleFoam with RNGkepsilon goes well and the result also improved. But the simpleFoam with RSM still can not get convergence. The time step continuity errors goes up after 20 timesteps. I upload the fvscheme, fvsolution and the log of the computational process. What is your opinion? beauty 

September 15, 2010, 04:16 

#12 
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 8 
Hi beauty,
i have the same problem. my lower turbulencemodels convergence very well. but my rsm does only convergence with the linearUpwindV cellLimited Gauss linear 1, but i get poor results with this schemes. i try to simulate a rotating swirl and read that the poor results reveal of the upwindscheme. i try to start the rsmmodell with a convergence kEpsilon flow as the startsetting and change some settings in the fvSolutionfile like GAMG instead of PCG and decrease the relaxationFactors for k,epsilon,R to 0.1. To you got any solutions? 

September 15, 2010, 10:33 

#13 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
First of all run checkMesh on your grid. If results are very poor with a second order discretization in RANS cases, you either have some mistake in the setup or a poor mesh.
Additionally, I think I missed beauty's post, however this div(phi,R) Gauss linear corrected; should be made consistent with the other convective terms. Finally, the underrelaxation factor for R could be lowered to 0.2, to help the solution in the initial stages. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 15, 2010, 10:36 

#14  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Quote:
Quote:
However it is difficult to answer without seeing the case setup. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 16, 2010, 03:49 

#15 
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 8 
Hi Alberto,
i believe that my results are diffuse. But I'm confused my results with the kEpsilonmodell are quiet better than the results of the RSTM modells (LRR and LaunderGibsonRSTM) when i use the linearUpwindVscheme. I run also checkMesh: Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 278866 faces: 819571 internal faces: 799079 cells: 269775 boundary patches: 5 point zones: 0 face zones: 1 cell zones: 1 Overall number of cells of each type: hexahedra: 269775 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology WALL 15091 15161 ok (nonclosed singly connected) IN 165 192 ok (nonclosed singly connected) OUT 1276 1321 ok (nonclosed singly connected) Tauchrohr 1320 1408 ok (nonclosed singly connected) TauchrohrINNEN 2640 1408 multiply connected (shared edge) <<Writing 1408 conflicting points to set nonManifoldPoints Checking geometry... Overall domain bounding box (0.2 0.145 1.305) (0.145 0.145 0.87) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (2.13432e17 2.41336e17 1.43938e16) OK. Max cell openness = 2.34986e16 OK. Max aspect ratio = 140.666 OK. Minumum face area = 8.17877e07. Maximum face area = 0.000644372. Face area magnitudes OK. Min volume = 1.587e08. Max volume = 3.82408e06. Total volume = 0.0992571. Cell volumes OK. Mesh nonorthogonality Max: 86.5265 average: 6.78598 *Number of severely nonorthogonal faces: 585. Nonorthogonality check OK. <<Writing 585 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 1.35194 OK. Mesh OK. End boundaries: I use for nut, k, epsilon,R wallfunctions. For the pressureoutlet i set outletInlet, outletValue uniform 0, value unifrom 5. I also uploaded my systemfile. regards. 

September 21, 2010, 05:40 

#16 
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 8 
Hi Foamers,
i refresh my mesh up to 3,6 mio cells and i still have convergence problems. There are also very high Penumbers in the range of 5000. I set for the velocityboundary 10 m/s and for the vicosity 1,6675e05. I think its very hard to lower the Pecletnumber with this setting. In my opinion 3,6 mio cells and more are to much to handle the problem with my pc. I figured out, that the i ought use max. 400.000 cells. I read a few of papers and the authors had no problems with fluent and the linearschemes for RSM and a mesh with 250.000 cells. 

September 21, 2010, 13:33 

#17 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
The problem is hardly the number of cells in your case but the case setup, and there we can be of no help without a case that reproduces the problem.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 24, 2010, 03:09 

#18 
New Member
Join Date: Mar 2010
Posts: 13
Rep Power: 8 
You're right Alberto.
I uploaded my setup. http://rapidshare.com/files/42091842...AM_cyclone.rar I hope anybody can get me some useful hints. kind regards! 

September 24, 2010, 17:21 

#19 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
You are actually using the linear scheme for div(phi, U), which might explain the poor convergence/results on a coarse mesh.
Try using the attached files, starting from the original initial condition (do not patch what you get from keps).
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 26, 2010, 07:50 

#20 
New Member

Hi，
I am glad to see the discussion on the problem of RSM here! Hi, spej, are you simulating the swirl flow in a cyclone? When simulating the flow in a cyclone, I can not get convergence by using RSM model. Maybe I have the setup problem. Next I will try alberto’s advice, and hope for better results! beauty 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Suggested unsteady, implicit solver stable with arbitrarily large time steps  djbungee  OpenFOAM Programming & Development  45  March 23, 2015 05:14 
Laminar simpleFoam and inviscid simpleFoam  herenger  OpenFOAM Running, Solving & CFD  7  July 11, 2013 06:27 
[Domain]Three different Domain  Young  CFX  3  April 27, 2008 14:11 
CFX Solver Memory Error  mike  CFX  1  March 19, 2008 08:22 
Diverging wall scale due to large domain size  Kevin  CFX  3  November 12, 2006 16:48 