CFD Online Discussion Forums - buoyantSimpleFoam and watertank

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - buoyantSimpleFoam and watertank (https://www.cfd-online.com/Forums/openfoam-solving/125718-buoyantsimplefoam-watertank.html)

Unfortunately I do not get beyond 0.07 seconds before the pressure blows up. If have attached the new version with the modified Allrun script. Switching off the turbulence does not make any difference...

I am able to run that case if I change the BCs for p_rgh for bottom and wall to buoyantPressure and the one for top to fixedValue. Additionally I use funkySetField to initialize p. I have to use a lot of outerCorrectors (~30) at the beginning and underrelaxation, especially for p_rgh.

The velocity profile at the wall, due to the heat loss, is not as distinctive as before with buoyantBoussinesqPimpleFoam (see post #36). While the velocity profile is well developed in the lower region (after 360 sec), there are some disturbances in upper region probably caused by the BC for the top face.
Attachment 27962 Attachment 27963 Attachment 27964 Attachment 27965
At least the temperature distribution is stable and quite uniform in radial direction (except at the outer wall with the heat flux) which was previously not the case.

Does anyone have an idea which BCs might be as well appropiate for a closed tank?
Even though the case is running with the current BCs, it is probably a wrong setup since there is still some velocity (see Fig. 2, UY) at the top face where it should actually be zero...

Hi Bernhard,

I tryed several options.

- changing 0/ files
- changing initialization
- changing thermodynamicProperties (with air its working)

- test case with cht
- test case with buoyant
- test case with boussinesq

- testings with diverent meshes
- testings with several fvSolution options

- changing pEqn.H in buoyantPressure

- checking with laminar and turbulent flow characteristics

Summary:

- most simulations have a continuity problem (U_x,y,z) blow up and p_rgh too
- re-coarse the mesh did not solve the problem
- thermodynamics changing to perfectGas with air is working
- changing p_rgh (top) to fixedValue is working but the results are bad.

At the moment I am out of ideas - sorry.

Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...

Quote:

Originally Posted by BernhardS (Post 470256)

Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...

Additionally you can set g to (0 0 0)^T - it should give the same possibilty to solve the case but :D you need gravitation.

Quote:

Originally Posted by jherb (Post 461045)

Add the following line to your thermophysicalProperties:

Code:

dpdt no;

see:

[/code]

Hi all,

I might have an explanation of why the solution diverges when the density is non-constant and dpdt is on. I am hoping for your comments.

By using icoPolynomial we are setting the fluid as incompressible, i.e. $\rho(p,T) = \rho(T)$ . So we have, by definition:

$\frac{\partial\rho}{\partial p} = 0$

Which is what icoPolynomial returns when the function psi is called. For an ideal gas $\frac{1}{RT}$ is returned. The compressibility can be expanded to

$\frac{\partial\rho}{\partial t} \frac{\partial t}{\partial p} = 0$

or

$\frac{\partial\rho}{\partial t}\left[ \frac{\partial p}{\partial t}\right]^{-1} =0$

So if we have non constant density, $\frac{\partial\rho}{\partial t} \ne 0$ and hence $\frac{\partial p}{\partial t}$ must diverge?

Perhaps we would need and compressiblePolynomial class where the compressibility can be set even though it's really small for water?

Any thoughts?

Cheers
Nicolas

Hi Bernhard,
I'm facing a similar problem when I try to use icoPolynomial in a closed cavity. Could you solve your case?

Hi,

What kind of boundary conditions did you use? Could you be so nice and tell me which BC you used for the simulation with buoyantSimpleFoam, specially p and p_rgh. I am confused about these BC. I have changed the solver as recommended by Tom in the post.

Have a nice weekend,

MK.

Quote:

Originally Posted by Tobi (Post 460448)

Hi all,

now the pressure fields are the same (buoyantSimpleFoam and chtMultiRegionSimpleFoam) .

I had to change the schemes to get the same results :)

Now I am going to check if its working wit a bigger domain.

hi
I have continuity error with buoyantSimpleFoam :(
how did you change the schemes?
thanks

BuoyantPimpleFoam crashes when using polynomial thermophysical properties

Hi everyone,

I am using OpenFOAM 4-1 and I would like to run the buoyantPimpleFoam tutorial "hotroom" with the polynomial properties. The problem is the same as many of you got earlier which is that the solver crashed after few iterations (here 1 ...) and which is the following:

Quote:

I have followed the different advices given in this thread like:
*refining the mesh
*changing the pressure initialization in the solver or using funkySetFields to initialize the pressure
*modifying the relaxation factors in the fvSolution as well as increasing the number of inner and outer correctors
*using dpdt off/no

However, none of these solutions was solving my problem.

Has someone already had this problem before and solved it? Or do you have other any trick I could try to make it work?

Many thanks,

Antoine

Dear Antionio,

please start with dt = 1e-7. You first time step is too big and therefore the courant number explodes already: Courant Number mean: 9.24507 max: 26.4701. That would be my first guess. Especially because you run in PISO mode

Code:

PIMPLE: Operating solver in PISO mode

Thanks for your quick answer Tobi.

Yes I tried this as well and the solver crashes during the third time step. Here is the log file.

Quote:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.1
Exec : buoyantPimpleFoam
Date : Feb 07 2017
Time : 15:16:35
Host : "workstation"
PID : 30239
Case : /home/antoine/OpenFOAM/antoine-4.1/run/heatTransfer/buoyantPimpleFoam/hotRoom
nProcs : 1
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

PIMPLE: Operating solver in PISO mode

Reading thermophysical properties

Selecting thermodynamics package
{
type heRhoThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
energy sensibleEnthalpy;
equationOfState icoPolynomial;
specie specie;
}

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type laminar

Reading g

Reading hRef
Calculating field g.h

Reading field p_rgh

Creating field dpdt

Creating field kinetic energy K

No MRF models present

Radiation model not active: radiationProperties not found
Selecting radiationModel none
No finite volume options present

Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 1.2e-10
Time = 1.2e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.66064e-19, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for h, Initial residual = 0.0546701, Final residual = 1.0306e-22, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00887971, No Iterations 77
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.05398e-16, global = 3.9305e-17, cumulative = 3.9305e-17
DICPCG: Solving for p_rgh, Initial residual = 0.491793, Final residual = 0.00240797, No Iterations 75
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.4897e-16, global = 4.3335e-17, cumulative = 8.264e-17
DICPCG: Solving for p_rgh, Initial residual = 0.57848, Final residual = 0.00314953, No Iterations 75
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.4878e-16, global = 4.3335e-17, cumulative = 1.25975e-16
DICPCG: Solving for p_rgh, Initial residual = 0.586074, Final residual = 8.47746e-09, No Iterations 155
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.38492e-16, global = 4.4141e-17, cumulative = 1.70116e-16
ExecutionTime = 0.12 s ClockTime = 0 s

Courant Number mean: 5.2325e-16 max: 2.01354e-14
deltaT = 1.44e-10
Time = 2.64e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.375238, Final residual = 5.06174e-17, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.425447, Final residual = 1.02992e-16, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.376789, Final residual = 9.52503e-17, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.109804, Final residual = 2.35794e-17, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.95771, Final residual = 12.2972, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.12464e-13, global = -7.97004e-17, cumulative = 9.04156e-17
DICPCG: Solving for p_rgh, Initial residual = 0.969428, Final residual = 0.00897822, No Iterations 8
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.06168e-14, global = -8.09331e-17, cumulative = 9.4825e-18
DICPCG: Solving for p_rgh, Initial residual = 0.725705, Final residual = 0.00585134, No Iterations 11
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.01544e-14, global = -8.03642e-17, cumulative = -7.08817e-17
DICPCG: Solving for p_rgh, Initial residual = 0.705409, Final residual = 1.3606, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.04522e-14, global = -8.13598e-17, cumulative = -1.52242e-16
ExecutionTime = 0.36 s ClockTime = 0 s

Courant Number mean: 8.14634e-14 max: 2.0581e-13
deltaT = 1.728e-10
Time = 4.368e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.389284, Final residual = 6.39416e-16, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.374786, Final residual = 6.94543e-17, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.636027, Final residual = 1.45355e-16, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.996707, Final residual = 6.67237e-16, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.808542, Final residual = 1.16481e+09, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000418179, global = -2.55172e-13, cumulative = -2.55324e-13
DICPCG: Solving for p_rgh, Initial residual = 0.999999, Final residual = 0.00614212, No Iterations 13
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 2.56852e-06, global = -2.55169e-13, cumulative = -5.10493e-13
DICPCG: Solving for p_rgh, Initial residual = 0.99982, Final residual = 0.00569006, No Iterations 14
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.46772e-08, global = -2.55171e-13, cumulative = -7.65664e-13
DICPCG: Solving for p_rgh, Initial residual = 0.96881, Final residual = 4.72076, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.21886e-08, global = -2.5517e-13, cumulative = -1.02083e-12
ExecutionTime = 0.61 s ClockTime = 0 s

Courant Number mean: 1.41177e-07 max: 3.2514e-07
deltaT = 2.0736e-10
Time = 6.4416e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.376711, Final residual = 2.2168e-15, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.412434, Final residual = 2.2696e-15, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.420672, Final residual = 2.49295e-15, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 6.01906e-15, No Iterations 1

--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hPolynomialThermo<Foam::icoPolynomial<Foam:: specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hPolynomialThermo<Foam ::icoPolynomial<Foam::specie> >, Foam::sensibleEnthalpy>]
in file /home/antoine/OpenFOAM/OpenFOAM-4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() at ??:?
#3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Aborted (core dumped)

Many thanks,

Antoine

Your p_rgh solver has problems:

Code:

DICPCG: Solving for p_rgh, Initial residual = 0.95771, Final residual = 12.2972, No Iterations 1001

You should use GAMG solver for pressure (speed up)
However, this will not solve your problem
Mesh problem
But I think you have a BC problem

Good luck,

Thanks for your advice Tobias. I will investigate.

Cheers,

Antoine

Dear All,

In case some of you are interested, the problem was while using polynomial density or boussinesq approximation in the case of a closed volume with buoyantPimpleFoam. The bug was reported and corrected in the lastest version of OpenFOAM-dev. (https://bugs.openfoam.org/view.php?id=2617)

Best regards,

Antoine

Hi All,

I know this is a bit of an old thread but I'm struggling with the exact same issue as Tobi did, namely when I try to simulate a hot water jet entering a large body of water with polynomial equations for state my density solution exceeds the maximum no. iterations. I'd like to simulate something similar to this thesis:
http://www.diva-portal.org/smash/get...421/FULLTEXT01

I gather it's the polynomials themselves that are causing the issue but I'm clueless as to how to fix this. Does anyone have any successful example cases for such a problem?

Funnily enough, my case works fine with buoyantBoussinesqSimpleFoam.

Thanks,

Artur

Hi!

Which version are you using? I think the bug I mentioned in a previous post was corrected in OpenFOAM 4.x.

Otherwise is the term dpdt set to off or no in your thermophysical file?

Regards,

Antoine

Hi,
Thanks for the prompt reply. I'm using 5.0 and at the moment not, I didn't have the unsteady term switched off. I'll try to see how to do it but if you could let me know that would also be great :)
Artur

EDIT: okay, just tried and it didn't change anything. I also tried to fix the density, viscosity, kappa and Cp by setting the constant term of the polynomials to the correct value and the rest to zero but to no avail.

EDIT 2: I posted my case with the mesh here, if anyone who knows more about this category of solvers would like to have a look it'd be much appreciated!
https://www.dropbox.com/s/b4hu90ajdn...le.tar.gz?dl=0

Hi All,

After some intense figuring out and help from Antoine I managed to get the case working. The trick seems to be in using a temperature and velocity limiter for the first few iterations to allow the solver to cope with the admittedly complicated BC set up that my case has. You just need to put the attached fvOptions file in the constant directory and then comment the limiters out later on (or just make sure the limits have a sensible margin in the first place I guess).

All the best,

A

Attachment 64157

Hi,

Just one question. Do you start with a steady state solver?