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

Heattransfer of a pipe using chtMultiRegionFoam

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 25, 2014, 12:19
Default
  #21
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 12
skuznet is on a distinguished road
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

Code:
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!
Attached Images
File Type: jpg SolidFluidT.jpg (37.7 KB, 40 views)
File Type: jpg FluidU.jpg (45.8 KB, 29 views)
File Type: jpg SolidT.jpg (37.9 KB, 29 views)
skuznet is offline   Reply With Quote

Old   March 25, 2014, 12:47
Default
  #22
Member
 
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 15
zhengzh5 is on a distinguished road
Quote:
Originally Posted by skuznet View Post
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

Code:
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:

Code:
U
inlet fixedValue;
outlet zeroGradient/inletOutlet;

p_rgh
inlet zeroGradient;
outlet fixedValue;
to use polynomial thermophysical properties, your thermophysicalProperties would have the following format:

Code:
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

Code:
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

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

        smoother         GaussSeidel;

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

Code:
    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.
zhengzh5 is offline   Reply With Quote

Old   August 5, 2014, 05:42
Default
  #23
Senior Member
 
Laurent DASTUGUE
Join Date: May 2014
Location: Chartres, France
Posts: 122
Rep Power: 12
laurentD is on a distinguished road
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
laurentD is offline   Reply With Quote

Old   October 24, 2016, 11:00
Default
  #24
Senior Member
 
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10
manuc is on a distinguished road
Dear Laurent

Were you able to solve the issue. I have a geometry of packed spheres and looking for natural convection flow.
__________________
Regards
Manu
manuc is offline   Reply With Quote

Old   February 17, 2017, 16:33
Default
  #25
New Member
 
Join Date: Nov 2016
Posts: 8
Rep Power: 9
Bob! is on a distinguished road
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.
Bob! is offline   Reply With Quote

Reply

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
[DesignModeler] DesignModeler Pipe within pipe shields ANSYS Meshing & Geometry 13 November 25, 2018 22:14
Heattransfer between two fluids with chtMultiRegionFoam Black-Pearl OpenFOAM Running, Solving & CFD 1 September 7, 2013 08:03
fluid to solid heattransfer with chtMultiRegionFoam schteff OpenFOAM 5 August 20, 2010 07:45
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 15:31.