
[Sponsors] 
Heattransfer of a pipe using chtMultiRegionFoam 

LinkBack  Thread Tools  Search this Thread  Display Modes 
March 25, 2014, 12:19 

#21 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 12 
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 = 2.680873e07, Final residual = 2.28762e09, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 5.500761e07, Final residual = 4.011625e09, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 4.513433e07, Final residual = 3.936525e09, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 6.467982e05, Final residual = 5.163352e06, No Iterations 1 Min/max T:300 496.1213 GAMG: Solving for p_rgh, Initial residual = 1.589845e06, Final residual = 3.968826e07, No Iterations 1000 time step continuity errors : sum local = 8.038446e07, global = 3.182782e09, cumulative = 72.02389 Min/max rho:1000 1000 Solving for solid region solidSmall DICPCG: Solving for h, Initial residual = 6.506662e05, Final residual = 3.32728e07, 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 steadystate cases and how do I choose BC for turbulence fields? Thanks for helping me with it! 

March 25, 2014, 12:47 

#22  
Member
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 15 
Quote:
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; 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 1.11868e1 5.45205e4 1.23115e6 1.34899e9 5.85372e13 0); Hf 0; //2246832; Sf 0; } transport { muCoeffs<8> (2.10656e1 3.28622e3 2.13578e5 7.35798e8 1.41336e10 1.43336e13 5.99260e17 0); kappaCoeffs<8> (7.06477e2 3.91625e3 2.51734e5 8.03261e8 1.42640e10 1.35149e13 5.33213e17 0); } equationOfState { rhoCoeffs<8> (9.844e2 1.55703 4.23397e3 1.13545e5 1.81906e8 1.69339e11 7.13007e15 0); } } 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 Code:
p_rgh { solver GAMG; tolerance 1e7; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } Code:
p_rgh { solver PCG; preconditioner DIC; tolerance 1e7; relTol 0.01; } 

August 5, 2014, 05:42 

#23 
Senior Member
Laurent DASTUGUE
Join Date: May 2014
Location: Chartres, France
Posts: 122
Rep Power: 12 
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 steadystate 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 

October 24, 2016, 11:00 

#24 
Senior Member
Manu Chakkingal
Join Date: Feb 2016
Location: Delft, Netherlands
Posts: 129
Rep Power: 10 
Dear Laurent
Were you able to solve the issue. I have a geometry of packed spheres and looking for natural convection flow.
__________________
Regards Manu 

February 17, 2017, 16:33 

#25 
New Member
Join Date: Nov 2016
Posts: 8
Rep Power: 9 
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. 

Thread Tools  Search this Thread 
Display Modes  


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  BlackPearl  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 