[Tobi]

Dear all,

switching from kEpsilon into kOmegaSST in the tutorial (compressible/rhoSimpleFoam) you will get the following error while starting the solver:

Selecting RAS turbulence model kOmegaSST


--> FOAM FATAL ERROR: 
Arguments of min have different dimensions
     dimensions : [0 -2 2 0 0 0 0] and [0 0 0 0 0 0 0]


    From function min(const dimensionSet&, const dimensionSet&)
    in file dimensionSet/dimensionSet.C at line 239.

FOAM aborting

Regards Tobi

[ngj]

Good evening Tobias,

I suppose that you copied epsilon upon making the file omega to adapt to the kOmegaSST solver? In that process you forgot that omega and epsilon do not have the same dimensions. Correct the dimensions in omega and you should be able to run the case (after adjusting fvSchemes and fvSolution as well).

Kind regards

Niels

[Tobi]

Originally Posted by ngj

Good evening Tobias,

I suppose that you copied epsilon upon making the file omega to adapt to the kOmegaSST solver? In that process you forgot that omega and epsilon do not have the same dimensions. Correct the dimensions in omega and you should be able to run the case (after adjusting fvSchemes and fvSolution as well).

Kind regards

Niels

Hi niels,

well I am so stupid

Thanks for the hint.

[ghtunmun]

Hello dear foamers,
I hope someone can help me!
I'm using OF2.2.x and I'm trying to run the tutorial case of rhoSimpleFoam with kOmegaSST:
Well to do that
1) I changed my RAS properties
2) I created an omega file with the functions "compressible:megaWallFunction" and "compressible::turbulentMixingLengthFrequencyInlet "
3) I replaced the epsilon with omega in fvSchemes and fvSolution
But the problem is that my simulation crashes after only 3 timesteps with this error:

Time = 3

smoothSolver: Solving for Ux, Initial residual = 0.0240306, Final residual = 0.00026193, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.0599666, Final residual = 0.000503615, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.269707, Final residual = 0.0221852, No Iterations 2
DILUPBiCG: Solving for e, Initial residual = 0.120954, Final residual = 0.00439071, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 Uninterpreted:
#3 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() at ??:?
#4 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() at ??:?
#5
at ??:?
#6 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#7
at ??:?

I also tried with sensibleEnthalpy instead of sensibleInternalEnergy in thermophysicalproperties but I get the same errors after the second timestep
Do you have an idea how i can fix this problem? I would be very grateful if you can help me!
Thanks

[Tobi]

Originally Posted by ghtunmun

Hello dear foamers,
I hope someone can help me!
I'm using OF2.2.x and I'm trying to run the tutorial case of rhoSimpleFoam with kOmegaSST:
Well to do that
1) I changed my RAS properties
2) I created an omega file with the functions "compressible:megaWallFunction" and "compressible::turbulentMixingLengthFrequencyInlet "
3) I replaced the epsilon with omega in fvSchemes and fvSolution
But the problem is that my simulation crashes after only 3 timesteps with this error:
I also tried with sensibleEnthalpy instead of sensibleInternalEnergy in thermophysicalproperties but I get the same errors after the second timestep
Do you have an idea how i can fix this problem? I would be very grateful if you can help me!
Thanks

What is the output of the first two timesteps?

[ghtunmun]

Hi Tobi,
thanks for answering this is all what I get:

Create time

Create mesh for time = 0


SIMPLE: convergence criteria
field p tolerance 0.01
field U tolerance 0.0001
field e tolerance 0.001
field "(k|omega)" tolerance 0.001

Reading thermophysical properties

Selecting thermodynamics package
{
type hePsiThermo;
mixture pureMixture;
transport sutherland;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
Prt 1;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

Creating finite volume options
Creating fintite volume options from fvOptions

Selecting finite volume options model type fixedTemperatureConstraint
Source: fixedTemperaure1
- applying source for all time
- selecting cells using cellZone porosity
- selected 8000 cell(s) with volume 0.00025

Selecting finite volume options model type explicitPorositySource
Source: porosity1
- applying source for all time
- selecting cells using cellZone porosity
- selected 8000 cell(s) with volume 0.00025

Porosity region porosity1:
selecting model: fixedCoeff
creating porous zone: porosity

Starting time loop

Time = 1

smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0707905, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.063064, No Iterations 4
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0677523, No Iterations 4
DILUPBiCG: Solving for e, Initial residual = 0.00130693, Final residual = 2.3513e-05, No Iterations 1
GAMG: Solving for p, Initial residual = 1, Final residual = 0.0200219, No Iterations 6
time step continuity errors : sum local = 2.72809, global = 0.175159, cumulative = 0.175159
rho max/min : 1.20199 1.1863
smoothSolver: Solving for omega, Initial residual = 0.084746, Final residual = 0.00225388, No Iterations 4
smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.0643399, No Iterations 4
ExecutionTime = 0.86 s ClockTime = 1 s

Time = 2

smoothSolver: Solving for Ux, Initial residual = 0.998206, Final residual = 0.0203196, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.906368, Final residual = 0.0162793, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.463741, Final residual = 0.00948249, No Iterations 2
DILUPBiCG: Solving for e, Initial residual = 0.0733407, Final residual = 0.00241027, No Iterations 1
GAMG: Solving for p, Initial residual = 0.0922751, Final residual = 0.00371497, No Iterations 3
time step continuity errors : sum local = 803.37, global = 3.709, cumulative = 3.88416
rho max/min : 1.21689 1.18597
smoothSolver: Solving for omega, Initial residual = 0.916676, Final residual = 0.0167419, No Iterations 4
bounding omega, min: -19480.4 max: 1.52032e+06 average: 40535.1
smoothSolver: Solving for k, Initial residual = 0.972079, Final residual = 0.0405412, No Iterations 2
ExecutionTime = 1.19 s ClockTime = 1 s

Time = 3

smoothSolver: Solving for Ux, Initial residual = 0.0239721, Final residual = 0.000260599, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.0595751, Final residual = 0.000499707, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.267433, Final residual = 0.0219196, No Iterations 2
DILUPBiCG: Solving for e, Initial residual = 0.118675, Final residual = 0.00436281, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 Uninterpreted:
#3 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() at ??:?
#4 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() at ??:?
#5
at ??:?
#6 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#7
at ??:?

[Tobi]

Originally Posted by ghtunmun

Hi Tobi,
thanks for answering this is all what I get:

Hi.

1. I prefer to use DILUPBiCG instead of smooth solver
2.

smoothSolver:  Solving for omega, Initial residual = 0.916676, Final residual = 0.0167419, No Iterations 4
bounding omega, min: -19480.4 max: 1.52032e+06 average: 40535.1

extrem bounding problem.
Have you set up your BC and initial conditions correct? It seems that there is something wrong.

3. write your timestep 1 and 2 out and have a look at those steps.
4. your relaxationsfactors?
5. did you use relaxationfactor in your fvSolution for omega? If not its set to 1

Check out 5 first

Regards Tobi

[ghtunmun]

Hey,
well it seems that the initial value that I chose for my internal field was causing this problem. I tried values as 1 or 5 or 10 and i still had those problems. But for values over 20 it seems to be running alright. I can't say too much about the results but the essential is that my simulation now runs and converges after 759 Iterations.

Thanks for your help!
Ghaith

[jvd.mechanic]

hi dear CFD users
who know this error that occur when i run "rhoSimpleFoam" to run my case and where i can find full description of solvers specially rhoSimpleFoam ?

Create time

Create mesh for time = 0


SIMPLE: convergence criteria
field p tolerance 0.01
field U tolerance 0.0001
field e tolerance 0.001
field "(k|epsilon|omega)" tolerance 0.001

Reading thermophysical properties

Selecting thermodynamics package
{
type hePsiThermo;
mixture pureMixture;
transport sutherland;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}

#0 Foam::error: :rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::heThermo<Foam: :siThermo, Foam: : ureMixture<Foam::sutherlandTransport<Foam::species ::thermo<Foam::hConstThermo<Foam: :erfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::init() at ??:?
#4 Foam::heThermo<Foam: :siThermo, Foam: : ureMixture<Foam::sutherlandTransport<Foam::species ::thermo<Foam::hConstThermo<Foam: : erfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::heThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#5 Foam::hePsiThermo<Foam: :siThermo, Foam: : ureMixture<Foam::sutherlandTransport<Foam::species ::thermo<Foam::hConstThermo<Foam: : erfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::hePsiThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#6 Foam: :siThermo::addfvMeshConstructorToTable<Foam::hePsi Thermo<Foam: : siThermo, Foam: : ureMixture<Foam::sutherlandTransport<Foam::species ::thermo<Foam::hConstThermo<Foam: : erfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#7 Foam::autoPtr<Foam: :siThermo> Foam::basicThermo::New<Foam: :siThermo>(Foam::fvMesh const&, Foam::word const&) at ??:?
#8 Foam: :siThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#9
at ??:?
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
at ??:?
Floating point exception (core dumped)


Thank you sincerely previously

[Tobi]

Hello Javad,

normally you get this early error if you set up something wrong in the 0/* files (I am not totaly sure if its there). The easiest way to solve the problem is the following:

1. copy existing rhoSimpleFoam tutorial to a place you want to work
2. run this tutorial case to see if everything is working well
3. copy your new generated mesh into the tutorial (polyMesh)
4. change the boundary in 0/* - just the names (do not modify with your own BC)
5. run this case
6. modify your BC in the files stored in 0/*
7. run this case again
8. modify other stuff (if it is necessary)
9. run this case again
10. .
11. .
12. .

After that you can compare the settings to your old one. Hence you have the ability to realize what was wrong.


I know that error, but unfortunatelly I am out of mind what cause this error. Maybe a missing entry in 0/* files:

value uniform x;

Hope this schedule will help you.
It is appreciated to get a feedback (:

PS: With the following code you can compare your files:

diff --help

[jvd.mechanic]

hi Tobi
thank you for your answer
I'm glad that you answer my question :-)

[jvd.mechanic]

hi every dear users an Tobi
I have a question in solving, can you help me?
I I've taken mesh of wingMotion to rhoSimpleFoam solver's folder to have a solve with certain conditions on the wing. with the basic initial values,the case run and doesn't problem but in high values of velocity ( high Reynolds ) ant turbulent situation ( I gave the values from CFD site ) solve has dump in 3th or 4th step.error occur in Energy equation
I reduce value of relaxationFactors for energy and the case solved for all time step.but decrement for relaxationFactors must be very high to dissolving : 10e-5 !!!!!!
can you help me how i can fix my case?

I'm in emergency situation, please help me if every person can

thank you

[Tobi]

Hi, well to help you without sufficient information is not easy... Is your mesh okay? Nonorthogonality?

Can you share your case? It would be good to have a look into your settings and mesh, bc schemes etc.

Regards
Tobi

[jvd.mechanic]

Originally Posted by Tobi

Hi, well to help you without sufficient information is not easy... Is your mesh okay? Nonorthogonality?

Can you share your case? It would be good to have a look into your settings and mesh, bc schemes etc.

Regards
Tobi

Hi
Definitely
the sharing address :
http://wikisend.com/download/856110/...fFixed1.tar.gz

I must say that the field of U has 2 bugs ; pls fixed them then run the case(Although the results will not change much) :
1.internalField uniform (0 0 0)
2.inlet
{
type flowRateInletVelocity;
massFlowRate constant 103;
value uniform (264 0 0);

thanks a lot

[Tobi]

Hi,

I downloaded your case and had a look at it. There are several points to say:

• your velocity goes up to 390 m/s on the freestream side. Hence you consider that you will reach velocitys >> 390 m/s around the airfoil. That is Ma > 1 and I am not sure if you can solve this problem with rhoSimpleFoam

• If you set a slip BC then you should also use the boundary type slip in constant/polyMesh/boundary

• I prefer to use PBGCi and DILU for U

• If you have a high velocity field you should switch on the transonic calculation in the pressure equation

  SIMPLE transonic   true;

• For pressure you should use PBGCi too

• Play with BC for sonic flow or stuff like that (not only fixedValue)

• Have a look into sonicFoam -> airfoil

• maybe sonicFoam is the better choice

• initial your field with potentialFoam

• check your turbulence properties for your INLET

At least maybe some interesting hints after some disscussion with a good openfoam`er friend:

• If rhoSimpleFoam is not working you should change to rhoPimpleFoam or transient solver because some times the physical prediction in steady-state solver could be wrong (in time) and could produce unphysical results
  
  This phenomena I got yesterday, the flow information in the outer region were faster than in the mid-area. Therefor a transient solver could be a good solution

At the moment your case is running but without changing in p-field