[skuznet]

Jace,

Thank you for you reply.

1. the size is 1.2x1.2x0.6 meter, so i takes about 12 second to flow through the domain. This is small time and fluid obviously cann't heat up to the large temparatures, howver my concern is that temperature distribution is not symmetric. There are temperature concentrations, distributed not symmetrically.

I just run this case with initial fluid velocity 0.001 and the results from temperature distribution improved, not it looks realistic (see the picture attached).
However with such a small velocity I've problems with convergence for p_rhg - it takes 1000 iterations each step

Time = 2024


Solving for fluid region fluidSmall
DILUPBiCG:  Solving for Ux, Initial residual = 2.680873e-07, Final residual = 2.28762e-09, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 5.500761e-07, Final residual = 4.011625e-09, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 4.513433e-07, Final residual = 3.936525e-09, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 6.467982e-05, Final residual = 5.163352e-06, No Iterations 1
Min/max T:300 496.1213
GAMG:  Solving for p_rgh, Initial residual = 1.589845e-06, Final residual = 3.968826e-07, No Iterations 1000
time step continuity errors : sum local = 8.038446e-07, global = -3.182782e-09, cumulative = -72.02389
Min/max rho:1000 1000

Solving for solid region solidSmall
DICPCG:  Solving for h, Initial residual = 6.506662e-05, Final residual = 3.32728e-07, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 500
ExecutionTime = 3685.64 s  ClockTime = 3691 s

I'm not sure why it happens. I would expect better convergence for smaller velocities.
The only think i can think of is that the pressure drop in p_rgh is too small compared to reference pressure (1e5).


2. thanks for suggesting it, I will try zeroGradient BC. I don't have enough experience in fluid dynamics, therefore it is not easy for me to chose right BCs.

3. I would like to use polynomial thermophysical properties in future, when I get comfortable with constant properties. Is any example available where I can see how to use polynomial properties? Do you have such a case?


4. Also I would like to introduce turbulence. Can you please suggest me which turbulence model I can use for transient and for steady-state cases and how do I choose BC for turbulence fields?


Thanks for helping me with it!

[zhengzh5]

Originally Posted by skuznet

Jace,

Thank you for you reply.

1. the size is 1.2x1.2x0.6 meter, so i takes about 12 second to flow through the domain. This is small time and fluid obviously cann't heat up to the large temparatures, howver my concern is that temperature distribution is not symmetric. There are temperature concentrations, distributed not symmetrically.

I just run this case with initial fluid velocity 0.001 and the results from temperature distribution improved, not it looks realistic (see the picture attached).
However with such a small velocity I've problems with convergence for p_rhg - it takes 1000 iterations each step

Time = 2024


Solving for fluid region fluidSmall
DILUPBiCG:  Solving for Ux, Initial residual = 2.680873e-07, Final residual = 2.28762e-09, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 5.500761e-07, Final residual = 4.011625e-09, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 4.513433e-07, Final residual = 3.936525e-09, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 6.467982e-05, Final residual = 5.163352e-06, No Iterations 1
Min/max T:300 496.1213
GAMG:  Solving for p_rgh, Initial residual = 1.589845e-06, Final residual = 3.968826e-07, No Iterations 1000
time step continuity errors : sum local = 8.038446e-07, global = -3.182782e-09, cumulative = -72.02389
Min/max rho:1000 1000

Solving for solid region solidSmall
DICPCG:  Solving for h, Initial residual = 6.506662e-05, Final residual = 3.32728e-07, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 500
ExecutionTime = 3685.64 s  ClockTime = 3691 s

I'm not sure why it happens. I would expect better convergence for smaller velocities.
The only think i can think of is that the pressure drop in p_rgh is too small compared to reference pressure (1e5).


2. thanks for suggesting it, I will try zeroGradient BC. I don't have enough experience in fluid dynamics, therefore it is not easy for me to chose right BCs.

3. I would like to use polynomial thermophysical properties in future, when I get comfortable with constant properties. Is any example available where I can see how to use polynomial properties? Do you have such a case?


4. Also I would like to introduce turbulence. Can you please suggest me which turbulence model I can use for transient and for steady-state cases and how do I choose BC for turbulence fields?


Thanks for helping me with it!

hey,

I still haven't quite get my head around the fixedFluxPressure BC yet, i usually just use zeroGradient for them, doesn't seem to be causing any trouble. for the inlet, try changing the p_rgh BC to zeroGradient.

so you would have:

U
inlet fixedValue;
outlet zeroGradient/inletOutlet;

p_rgh
inlet zeroGradient;
outlet fixedValue;

to use polynomial thermophysical properties, your thermophysicalProperties would have the following format:

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

dpdt no;

mixture
{
    specie
    {
        nMoles          1;
	molWeight 100.23;
    }
    thermodynamics
    {
      CpCoeffs<8> (1.63287e3 1.01615e1 -1.11868e-1 5.45205e-4 -1.23115e-6 1.34899e-9 -5.85372e-13 0);

      Hf 0; //-2246832;
      Sf 0;
    }
    transport
    {
      muCoeffs<8> (2.10656e-1 -3.28622e-3 2.13578e-5 -7.35798e-8 1.41336e-10 -1.43336e-13 5.99260e-17 0);
      kappaCoeffs<8> (-7.06477e-2 3.91625e-3 -2.51734e-5 8.03261e-8 -1.42640e-10 1.35149e-13 -5.33213e-17 0);

    }
    equationOfState
      {
	rhoCoeffs<8> (9.844e2 -1.55703 4.23397e-3 -1.13545e-5 1.81906e-8 -1.69339e-11 7.13007e-15 0);
      }
}

you have to find the coefficient for density, Cp, viscosity, and thermal conductivity for your fluid (water). the coefficients are arranged such that

CpCoeffs<8> (a1 a2 a3 a4 a5 a6 a7 a8);

where Cp = a1 + a2*T + a3*T^2 + a4*T^3 + a5*T^4 + a6*T^5 + a7*T^6 + a8*T^7

regarding the high iteration for p_rgh, I had that problem before too. I tried changing fvSolution from

    p_rgh
    {
        solver           GAMG;
        tolerance        1e-7;
        relTol           0.01;

        smoother         GaussSeidel;

        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator     faceAreaPair;
        mergeLevels      1;
    }

to

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-7;
        relTol   0.01;
}

it seems to drop that p_rgh iteration, but I haven't verify if it's causing any other issues...so you can try it out.

[laurentD]

Hi Stephan,
i'm trying to use 'chtmultiregionFoam' in my case (a radiator with a complex geometry) and i have exactly the same problem than yours.
I want to use kEpsilon model of turbulence and transient values of U and T in inlet of my model. But the job crashes saying to me : "maximum number of iterations exceeded ...etc" after a few iterations, even if i put a very little timestep.
I've tried too to initialize my job with some seconds of calculation with a steady-state flow and using 'chtMultiRegionSimpleFoam' but when i restart the job from the latest time with 'chtmultiregionFoam', i have the "maximum number of iterations exceeded..." message. It makes me crazy.
Have you solved your problem ?
If the answer is yes, what have you done?
Thank you for your reply.
Laurent

[manuc]

Dear Laurent

Were you able to solve the issue. I have a geometry of packed spheres and looking for natural convection flow.

[Bob!]

without having had that problem with that specific solver:

1) look in the terminal, which variable has too many iterations (last before error)

2) change the number of maximum iterations

3) if 2) doesen't work, change the " relaxationfactor" for that variable in fvSolution; you can give it a number between 0 and 1, lower number = less iteration

that was my solution in an other case.