CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM

Bounding Omega problems // Number of lambda iterations exceeds maxLambdaIter(10)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 7, 2022, 05:57
Default Bounding Omega problems // Number of lambda iterations exceeds maxLambdaIter(10)
  #1
New Member
 
Marie
Join Date: Mar 2022
Posts: 1
Rep Power: 0
Marie_Dal is on a distinguished road
Hello everyone,
I am new to OpenFoam. I am currently running a simulation of an airfoil using SimpleFoam with the turbulence model KomegaSST LM. After just a few iterations (4), the value of bounding omega (max) starts to be very high, which I believe is the reason why a warning appears a couple iterations after:

--> FOAM Warning :
From function Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> > Foam::RASModels::kOmegaSSTLM<BasicMomentumTranspor tModel>::ReThetat0(const Internal&, const Internal&, const Internal&) const [with BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::k inematicTransportModel>; Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Internal = Foam::DimensionedField<double, Foam::volMesh>]
in file ../momentumTransportModels/lnInclude/kOmegaSSTLM.C at line 300
Number of lambda iterations exceeds maxLambdaIter(10)

Now in my very little experience with this turbulence model, I believe this to be a boundary condition problem. I tried different values for omega, using wall functions for k, omega and nut, and also removing them, but nothing seems to work.

I tried turning my turbulence model back to the K omega SST, and the simulation runs without inconvenience, for which I assume the mesh is not the problem.

This is what an itertion with this warning looks like:

Time = 6

smoothSolver: Solving for Ux, Initial residual = 0.0493299, Final residual = 0.00422165, No Iterations 5
smoothSolver: Solving for Uy, Initial residual = 0.249744, Final residual = 0.0204515, No Iterations 4
GAMG: Solving for p, Initial residual = 0.107384, Final residual = 0.00826549, No Iterations 3
time step continuity errors : sum local = 0.000609625, global = -6.2441e-06, cumulative = -1.32525e-05
--> FOAM Warning :
From function Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> > Foam::RASModels::kOmegaSSTLM<BasicMomentumTranspor tModel>::ReThetat0(const Internal&, const Internal&, const Internal&) const [with BasicMomentumTransportModel = Foam::IncompressibleMomentumTransportModel<Foam::k inematicTransportModel>; Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Internal = Foam::DimensionedField<double, Foam::volMesh>]
in file ../momentumTransportModels/lnInclude/kOmegaSSTLM.C at line 300
Number of lambda iterations exceeds maxLambdaIter(10)
smoothSolver: Solving for ReThetat, Initial residual = 0.0628862, Final residual = 0.00492529, No Iterations 5
smoothSolver: Solving for gammaInt, Initial residual = 0.00826379, Final residual = 0.000491998, No Iterations 4
bounding gammaInt, min: -0.0724182 max: 1.11402 average: 0.963246
smoothSolver: Solving for omega, Initial residual = 0.0155426, Final residual = 0.00154728, No Iterations 6
bounding omega, min: -112.337 max: 2.47547e+10 average: 1.1801e+06
smoothSolver: Solving for k, Initial residual = 0.998501, Final residual = 7.2704e-05, No Iterations 1
ExecutionTime = 6.61 s ClockTime = 7 s




An error finally comes up after 18 iterations, when everything has already diverged:

Time = 18

smoothSolver: Solving for Ux, Initial residual = 0.730684, Final residual = 3.77352e+08, No Iterations 10
smoothSolver: Solving for Uy, Initial residual = 0.658047, Final residual = 3.8716e+08, No Iterations 10
#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:?
#4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#8 Foam::fvMatrix<double>::solve() in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#9 ? in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/simpleFoam"
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11 ? in "/opt/openfoam9/platforms/linux64GccDPInt32Opt/bin/simpleFoam"



I have faced very similar problems with other simulations, but changing boundary conditions (usually rising the value for omega) has always seemed to fix them. Yet, no matter what I try with this simulation, I can't seem to fix it.

I very much appreciate anyone's advice. I attach below boundary conditions and gradient schemes.

Thank you. :)

BOUNDARY CONDITIONS:

GammaInt:

internalField uniform 1;
boundaryField
{ inlet { type fixedValue;
value $internalField; }
outlet
{ type zeroGradient; }
walls
{ type zeroGradient; }
airfoil
{ type zeroGradient; }
frontAndBackPlanes
{ type empty; } }


K:
internalField uniform 0.00135;

boundaryField
{ inlet
{ type fixedValue;
value uniform 0.00135; }
outlet
{ type zeroGradient; }
airfoil
{ type fixedValue;
value uniform 1e-6; }
walls
{ type zeroGradient; }
frontAndBackPlanes
{ type empty; }}

nut
internalField uniform 0.0020125;

boundaryField
{ inlet { type freestream;
freestreamValue uniform 0.0020125; }

outlet { type freestream;
freestreamValue uniform 0.0020125; }

airfoil { type nutkWallFunction;
value uniform 0.00000020125; }

walls { type zeroGradient; }

frontAndBackPlanes { type empty; }}


OMEGA:
dimensions [0 0 -1 0 0 0 0];

internalField uniform 2.6708;

boundaryField
{ inlet { type fixedValue;
value $internalField; }

outlet { type zeroGradient; }

airfoil { type omegaWallFunction;
value $internalField; }

walls { type zeroGradient; }

frontAndBackPlanes { type empty; }}



ReThetaT
internalField uniform 1170.563958;
boundaryField
{ inlet { type fixedValue;
value $internalField; }

outlet { type zeroGradient; }

walls { type zeroGradient; }

airfoil { type zeroGradient; }

frontAndBackPlanes { type empty; }}

For U and P I use freeStream and no slip conditions on the airfoil, altough those boundary conditions are vastly tested and I am certain those are not the problem.
Marie_Dal is offline   Reply With Quote

Old   May 4, 2022, 20:47
Default Inquiry
  #2
New Member
 
Abdelrahman Kamaleldin
Join Date: Jan 2021
Posts: 6
Rep Power: 5
akamal1099 is on a distinguished road
Hello my friend
did you find a solution?? I am experiencing this problem now.
Thanks
akamal1099 is offline   Reply With Quote

Old   June 1, 2022, 06:34
Default
  #3
New Member
 
Emily
Join Date: Nov 2017
Posts: 24
Rep Power: 8
em17 is on a distinguished road
Hi, I am also having the exact same error. Has anyone managed to fix it?

Thanks, Em
em17 is offline   Reply With Quote

Old   June 1, 2022, 06:53
Default
  #4
New Member
 
Abdelrahman Kamaleldin
Join Date: Jan 2021
Posts: 6
Rep Power: 5
akamal1099 is on a distinguished road
Hello,
I did manage to fix it.
  1. Don't take y+ to be 1. Instead, take it to be >30 so you can use wall function for turbulence quantities
  2. I setted the inlet and outlet in one group and called it freestream
  3. Make sure you have the right boundary conditions for ReTheta and Gamma. You can check in openfoam wiki

I will upload my boundary files. But again I tried a lot to do the analysis with y+ = 1 but I couldn't. Some experts told me it a mesh problem even thought my mesh was fine per checkMesh. But there point was that if you are solving a 2D problem (only one cell in z direction throughout the whole mesh), the solver will experience such issues. So, I worked with y+>30 and I used wall fucntions

Hope it help.
Thanks
Attached Files
File Type: txt gammaInt.txt (1.3 KB, 56 views)
File Type: txt k.txt (1.4 KB, 35 views)
File Type: txt nut.txt (1.2 KB, 25 views)
File Type: txt omega.txt (1.4 KB, 40 views)
File Type: txt p.txt (1.2 KB, 16 views)
akamal1099 is offline   Reply With Quote

Old   June 1, 2022, 06:54
Default
  #5
New Member
 
Abdelrahman Kamaleldin
Join Date: Jan 2021
Posts: 6
Rep Power: 5
akamal1099 is on a distinguished road
Rest of files
Attached Files
File Type: txt ReThetat.txt (1.3 KB, 48 views)
File Type: txt U.txt (1.2 KB, 23 views)
akamal1099 is offline   Reply With Quote

Old   June 17, 2023, 22:06
Default
  #6
Senior Member
 
TWB
Join Date: Mar 2009
Posts: 402
Rep Power: 19
quarkz is on a distinguished road
Hi,

I have similar errors and my problem is an unsteady wing case in 3D.

For the bounding omega error, I change to:

Gauss linearUpwind default;

or

Gauss upwind;

For the maxLambdaIter error, my simulation continues to run w/o problem. But for subsequent simulations, I use:

kOmegaSSTLMCoeffs
{
maxLambdaIter 100;
}

You can give it a try to see if it works.
quarkz is offline   Reply With Quote

Old   July 17, 2023, 03:58
Default
  #7
New Member
 
Join Date: Jun 2023
Location: Brest
Posts: 21
Rep Power: 3
CFDUser29 is on a distinguished road
Also, it depends a lot on the conditions you impose.
For instance, if you do a quick sensibility study, you find that huge initial values for omega can bring erratic behavior to the residuals.

Also, it is interesting to look at the relaxation factor. For me, it is working well for 0.4 to 0.5, below it is too slow and add a lot of oscillations, and above (the value depends on the case you have), you can add bounding issues because you allow the solver to add a more important contributions for a given field in the equations where it contributes at each iteration.
CFDUser29 is offline   Reply With Quote

Reply

Tags
airfoil, komega sst model, komegasstlm

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Help sought on axial compressor simulation jyotir OpenFOAM Running, Solving & CFD 0 November 17, 2021 10:49
Problem with chtMultiregionFoam radiation boundary condition baran_foam OpenFOAM Running, Solving & CFD 10 December 17, 2019 17:36
Converging Diverging Nozzle with dbnsTurbFoam Saleh Abuhanieh OpenFOAM Running, Solving & CFD 4 December 13, 2019 10:26
chtMultiRegionSimpleFoam: maximum number of iterations excedeed. Nkl OpenFOAM Running, Solving & CFD 19 October 10, 2019 02:42
Free surface issues with interDyMFoam for hydroturbine oumnion OpenFOAM Running, Solving & CFD 0 October 6, 2017 14:05


All times are GMT -4. The time now is 15:05.