[rmz]

hello,
I am working on a simulation of wind on buildings with a complex Mesh.
I am using a RASModel kEspilon with the simpleFoam solver.
I am applying ABL conditions (atmospheric boundary layer).

I am facing problems with the solution convergence. the following is the begining of the output of simpleFoam:

Pstream initialized with:
floatTransfer : 0
nProcsSimpleSum : 0
commsType : nonBlocking
polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

Create time

Create mesh for time = 0

SIMPLE: convergence criteria
field p tolerance 0.001
field U tolerance 0.0001
field "(k|epsilon)" tolerance 0.0001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon

bounding k, min: 0 max: 46.975528397 average: 1.29999999999
bounding epsilon, min: 0 max: 173.377103808 average: 0.0100000000001
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.11;
C3 -0.33;
sigmak 1;
}

No MRF models present

No finite volume options present

and this is the end

Time = 1401

--> FOAM Warning :
From function Foam::fv::gaussConvectionScheme<Type>::gaussConvec tionScheme(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>]
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 124
Reading "/home/ingerop/OpenFOAM/ingerop-4.1/run_Dell/PAP_run/PAP_case_06_30/system/fvSchemes.divSchemes.div(phi,U)" at line 32
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/opt/openfoam4/etc/controlDict"
smoothSolver: Solving for Ux, Initial residual = 1.73686761346e-09, Final residual = 1.73686761346e-09, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 8.49670942582e-09, Final residual = 8.49670942582e-09, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 7.97749175341e-10, Final residual = 7.97749175341e-10, No Iterations 0
GAMG: Solving for p, Initial residual = 3.26294168382e-05, Final residual = 2.04903628538e-08, No Iterations 5
GAMG: Solving for p, Initial residual = 1.80088423459e-12, Final residual = 1.80088423459e-12, No Iterations 0
GAMG: Solving for p, Initial residual = 1.80088423459e-12, Final residual = 1.80088423459e-12, No Iterations 0
time step continuity errors : sum local = 1.92360928162e+41, global = -3.25979779589e+25, cumulative = -3.25979779589e+25
smoothSolver: Solving for epsilon, Initial residual = 2.08398503235e-17, Final residual = 2.08398503235e-17, No Iterations 0
smoothSolver: Solving for k, Initial residual = 8.88019064951e-08, Final residual = 7.39368688472e-11, No Iterations 5
bounding k, min: -6.88777988968e+34 max: 3.77003683949e+47 average: 1.86101835569e+41
ExecutionTime = 29170.4 s ClockTime = 29707 s

SIMPLE solution converged in 1401 iterations

End

Finalising parallel run

so my SIMPLE solution converged but I I have strange time step continuity error:
sum local = 1.92360928162e+41, global = -3.25979779589e+25, cumulative = -3.25979779589e+25

I am trynig to understand the meaning of "time step continuity errors". I searches the forum but didn't find a clear description.

What are the possible solutions to this problem.

thank you

[khedar]

Why don't you act on the warning issued by the solver,

Time = 1401

--> FOAM Warning : 
From function Foam::fv::gaussConvectionScheme<Type>::gaussConvec tionScheme(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>]
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 124
Reading "/home/ingerop/OpenFOAM/ingerop-4.1/run_Dell/PAP_run/PAP_case_06_30/system/fvSchemes.divSchemes.div(phi,U)" at line 32
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.

Try changing the scheme as suggested in the warning message and see if there is an improvement.


Also I see your k and epsilon are being bounded at before the actual start of the simulation itself. See here

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon

bounding k, min: 0 max: 46.975528397 average: 1.29999999999
bounding epsilon, min: 0 max: 173.377103808 average: 0.0100000000001
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.11;
C3 -0.33;
sigmak 1;
}

I would check the mesh using checkMesh and also check the boundary conditions for unrealistic values.

[rmz]

Hello Khedar,
thank you very musch for your answer.

-concerning the divScheme for (phi, U):
the old one was "Gauss limitedLinear 1".
I chaned it to "bounded Gauss limitedLinear 1".
I searched online and I found that this scheme could solve the time step continuity error.
Do you have any suggestions concerning the schemes?

-Concerning my mesh:
I checked my Mesh with the checkMesh utility and obtained bad results:

Checking geometry...
Overall domain bounding box (-2960 -3040 -0.121158714206) (3040 2960 300)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (2.17930274486e-17 -3.91561444179e-17 -1.08834515393e-15) OK.
Max cell openness = 5.38883049153e-16 OK.
Max aspect ratio = 34.3672506583 OK.
Minimum face area = 0.00067826511442. Maximum face area = 1142.7171814. Face area magnitudes OK.
Min volume = 9.51680068842e-05. Max volume = 13524.6338437. Total volume = 8480718988.88. Cell volumes OK.
Mesh non-orthogonality Max: 119.744918686 average: 17.8722895491
*Number of severely non-orthogonal (> 70 degrees) faces: 32644.
***Number of non-orthogonality errors: 3.
<<Writing 32647 non-orthogonal faces to set nonOrthoFaces
***Error in face pyramids: 41 faces are incorrectly oriented.
<<Writing 38 faces with incorrect orientation to set wrongOrientedFaces
***Max skewness = 18.9778817449, 1969 highly skew faces detected which may impair the quality of the results
<<Writing 1969 skew faces to set skewFaces
Coupled point location match (average 0) OK.

Failed 3 mesh checks.

End

I did a test simulation and replaced my geometry with just a box. SIMPLE converged without errors. so the mesh is the cause of the errors.

is there any utilities or parameters to change that can improve the mesh quality?

Also could you explain to me please which problems in the mesh are causing the bounding k and epsilon and why?

thank you for your help,
rmz

[rmz]

Hello,

I searched for schemes that can fix my bounding K and bounding epsilon problem.

I tried several simulations, and found a modification that improved my simulation:
changing "laplacianSchemes" from "Gauss linear limited 1" to Gauss linear limited 0.333
changing "snGradSchemes" from "limited 1" to limited 0.333

simpleFoam ran for 800 steps before the "bounding k" / "bounding epsilon" warning appears.

the following is an output from the last steps of simpleFoam:

Time = 2390

smoothSolver: Solving for Ux, Initial residual = 3.43286711522e-007, Final residual = 5.00656697633e-009, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 1.96835174901e-006, Final residual = 5.14760065778e-009, No Iterations 6
smoothSolver: Solving for Uz, Initial residual = 2.48971385257e-005, Final residual = 2.11086057017e-008, No Iterations 7
GAMG: Solving for p, Initial residual = 0.00550810426106, Final residual = 5.44662312053e-006, No Iterations 8
GAMG: Solving for p, Initial residual = 0.000618156877418, Final residual = 5.96389044258e-007, No Iterations 18
time step continuity errors : sum local = 3.24158762278e-010, global = -5.37971150415e-012, cumulative = 3.38998512783e-007
smoothSolver: Solving for epsilon, Initial residual = 9.37189059068e-008, Final residual = 3.66804560098e-011, No Iterations 6
bounding epsilon, min: 1.02539545302e-022 max: 2039304.52895 average: 383.995317993
smoothSolver: Solving for k, Initial residual = 8.19282585323e-007, Final residual = 5.03485913242e-010, No Iterations 10
bounding k, min: 3.00125902947e-016 max: 2992.53660103 average: 26.9353584992
ExecutionTime = 31197.191 s ClockTime = 31198 s

the problem of bounding k and epsilon is caused by skew faces in my mesh.
I am only interested in the results of p and U, and not interested in epsilon and k.
simpleFoam is stable and converging.

my question is:
-is simpleFoam converging to a correct solution (for p and U)?
-what is the accuracy of p and U results, does the bounding k and epsilon problem influence the results too much?

thank you

[khedar]

I would say its not right to assume that your results are good when you have bad values for some of your variables(k and Epsilon). You should definitely improve your mesh with respect to skewness. It looks very bad. One cannot stress enough on spending more time in creating a good quality mesh to avoid problems later on.