CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   simpleFoam convergence on large domain (http://www.cfd-online.com/Forums/openfoam/74618-simplefoam-convergence-large-domain.html)

kwiik April 5, 2010 03:46

simpleFoam convergence on large domain
 
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 zip-up check OK.
Face vertices OK.
Face-face 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 (1.04978e-15 9.99092e-15 6.43789e-14) OK.
Max cell openness = 3.74724e-16 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 non-orthogonality Max: 88.0021 average: 16.1696
*Number of severely non-orthogonal faces: 14.
Non-orthogonality check OK.
<<Writing 14 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 0.86499 OK.
All angles in faces OK.
All face flatness OK.

Mesh OK.

askjak April 6, 2010 10:09

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

beauty April 15, 2010 21:31

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 (non-closed singly connected)
inlet 96 119 ok (non-closed singly connected)
outlet 512 545 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.1 -0.15 -0.94) (0.0749999 0.0874996 0.4)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-4.04084e-19 -2.40544e-19 -1.16605e-19) OK.
Max cell openness = 3.73953e-16 OK.
Max aspect ratio = 134.96 OK.
Minumum face area = 1.6845e-08. Maximum face area = 0.000211397. Face area magnitudes OK.
Min volume = 2.10562e-10. Max volume = 6.46656e-07. Total volume = 0.0135334. Cell volumes OK.
Mesh non-orthogonality Max: 81.9702 average: 7.09614
*Number of severely non-orthogonal faces: 36.
Non-orthogonality check OK.
<<Writing 36 non-orthogonal 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 k-e model with upwind schemes(Divergence schemes), it works well. But after changing upwind to high-level schemes, it can't get convergence! what should I do to improve it?
Thanks!

alberto April 16, 2010 02:22

checkMesh is failing because you have highly skewed cells (and also some strongly non-orthogonal cell)

The second problem can probably be corrected indirectly with non-orthogonal correctors in the solver. For the first one, you've to re-consider the mesh.

Best,

beauty April 16, 2010 21:09

Hi, alberto

Thank you for your advice. I will rebuild my mesh and do my best to avoid skewed cells as well as non-orthogonal cells. If it works, I give a feekback.:p



beauty

beauty April 22, 2010 22:27

Hi,
The checkmesh result of my new mesh is as follows. The simplefoam with high-level schemes Still does not work. :mad:


Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
wall 6102 6143 ok (non-closed singly connected)
outlet 336 361 ok (non-closed singly connected)
inlet 72 90 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.1 -0.207 -0.86) (0.1 0.1 0.375)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-3.14905e-19 1.76981e-20 -7.25013e-19) OK.
Max cell openness = 3.11283e-16 OK.
Max aspect ratio = 35.1393 OK.
Minumum face area = 4.64258e-07. Maximum face area = 0.000339005. Face area magnitudes OK.
Min volume = 6.96387e-09. Max volume = 1.40468e-06. Total volume = 0.0216753. Cell volumes OK.
Mesh non-orthogonality Max: 81.1011 average: 7.28001
*Number of severely non-orthogonal faces: 18.
Non-orthogonality check OK.
<<Writing 18 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.77958 OK.

Mesh OK.

End


alberto April 23, 2010 00:18

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?

beauty April 23, 2010 03:22

2 Attachment(s)
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 "floating-point 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

alberto April 23, 2010 14:17

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,

beauty April 23, 2010 22:09

Hi, Alberto
Thanks for your timely reply, I will try as you suggest, I will upload result as soon as possible.

beauty

beauty April 24, 2010 03:43

RSM can not get convergence!
 
1 Attachment(s)
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 time-steps. I upload the fvscheme, fvsolution and the log of the computational process. What is your opinion?

beauty

spej September 15, 2010 04:16

Hi beauty,

i have the same problem. my lower turbulence-models 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 upwind-scheme. i try to start the rsm-modell with a convergence kEpsilon flow as the startsetting and change some settings in the fvSolution-file like GAMG instead of PCG and decrease the relaxationFactors for k,epsilon,R to 0.1.

To you got any solutions?

alberto September 15, 2010 10:33

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 under-relaxation factor for R could be lowered to 0.2, to help the solution in the initial stages.

Best,

alberto September 15, 2010 10:36

Quote:

Originally Posted by spej (Post 275264)
Hi beauty,

i have the same problem. my lower turbulence-models 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 upwind-scheme.

Does poor results mean very diffused?

Quote:

i try to start the rsm-modell with a convergence kEpsilon flow as the startsetting and change some settings in the fvSolution-file like GAMG instead of PCG and decrease the relaxationFactors for k,epsilon,R to 0.1.
The linear solver should not play any role, as long as the required convergence criterion is the same.

However it is difficult to answer without seeing the case setup.

Best,

spej September 16, 2010 03:49

1 Attachment(s)
Hi Alberto,

i believe that my results are diffuse. But I'm confused my results with the kEpsilon-modell are quiet better than the results of the RSTM modells (LRR and LaunderGibsonRSTM) when i use the linearUpwindV-scheme.

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 (non-closed singly connected)
IN 165 192 ok (non-closed singly connected)
OUT 1276 1321 ok (non-closed singly connected)
Tauchrohr 1320 1408 ok (non-closed 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 (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (2.13432e-17 2.41336e-17 1.43938e-16) OK.
Max cell openness = 2.34986e-16 OK.
Max aspect ratio = 140.666 OK.
Minumum face area = 8.17877e-07. Maximum face area = 0.000644372. Face area magnitudes OK.
Min volume = 1.587e-08. Max volume = 3.82408e-06. Total volume = 0.0992571. Cell volumes OK.
Mesh non-orthogonality Max: 86.5265 average: 6.78598
*Number of severely non-orthogonal faces: 585.
Non-orthogonality check OK.
<<Writing 585 non-orthogonal 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 pressure-outlet i set outletInlet, outletValue uniform 0, value unifrom 5.

I also uploaded my system-file.

regards.

spej September 21, 2010 05:40

Hi Foamers,
i refresh my mesh up to 3,6 mio cells and i still have convergence problems. There are also very high Pe-numbers in the range of 5000. I set for the velocity-boundary 10 m/s and for the vicosity 1,6675e-05. I think its very hard to lower the Peclet-number 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 linear-schemes for RSM and a mesh with 250.000 cells.

alberto September 21, 2010 13:33

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.

spej September 24, 2010 03:09

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!

alberto September 24, 2010 17:21

1 Attachment(s)
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 k-eps).

beauty September 26, 2010 07:50

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


All times are GMT -4. The time now is 23:59.