[manuc]

Hello all

I have tried to combine boussinesqPimlefoam and chtmultiregionfoam to get a solver
" boussinesqChtMultiRegionFoam ". I would like someone to have alook at it give suggestions and possible testcases to validate the same. I have used the following threads as a base for my development (especially the conjugate heat transfer coupling gin boundary condition).

http://www.cfd-online.com/Forums/ope...egionfoam.html

(the derived patch fields from the solver available in the above link was very slightly modified to suit my BC coupling need).

Please find the new solver at:
https://drive.google.com/file/d/0B6X...ew?usp=sharing

[Tobi]

Dear Manu,

I am not sure why you want to do this but in that case you just have to change the fluid momentum equation and add the Boussinesq approximation. Thats all. if you stuff is working is simple to verify. Use your new solver and solve the same case as you have in the Boussinesq solver. The results have to be similar.

[manuc]

Dear Tobi

As I understand you suggest to keep as foloows in the existing solver:
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState rhoConst;//perfectGas;
specie specie;
energy sensibleEnthalpy;
}

but modify the existing solver with

UEqn()
==
fvc::reconstruct
(
(
- ghf*fvc::snGrad(rhok)
- fvc::snGrad(p_rgh)
)*mesh.magSf()
),
mesh.solver(U.select(finalIter))


where
rhok = 1.0 - beta*(T - TRef);
--------------------------------------------------------
I would also like to add :
In chtmultiregionfoam if my solid region consists of 2 spheres in a fluid domain, is it possible to group the spheres so that I need to specify propertiess intitially for a single group (I have about 200 spheres)

[Tobi]

• First of all, please use code tags for code snippets
• You can not mix thermo physical models as you like to do, if you start your solver you should get an error and a list of possible options
• If you use a Boussinesq approximation, your fluid behaves incompressible and then you do not need any thermophysical database. You mix everything.

• Cht is for compressible and incompressible. You solve an energy equation and hence we need a thermophysical model.
• The solvers including a Boussinesq approximation does not solve any energy equation because we assume an incompressible fluid (we divide everything by the density). The buoyancy term is calculated with the Boussinesq approximation and added as a source term to the momentum equation

Please make sure that you do the correct things. Derive your equations and implement them or use the existing stuff from FOAM.

Good luck.

[manuc]

Dear Tobi
As per your suggestions I revisited my needs:

What do I need
1. A solver to carry out natural convection and mixed convection of fluids with solid bodies inside, resulting in a conjugate heat transfer
Why not chtmultiregion available at present with compressible eq. directly?
1.What I need to study is Prandtl number effect of fluids in conjugate heat transfer. Properties other than density doesnt change as per my assumption
2. The best-suited way to approach is Boussinesq assumption which is applicable for incompressible fluids.
What I tried
1.Modify the compressible flow equations in chtmultiregion solver. Replace it with incompressible momentum eq.
2. With the modification mentioned above I would be able to us transport proerties dictionary as in bouyantBoussinesqFoam and the thermo physical properties neednt be specified.
3. What I have now is an incompressible flow solver with boussinesq assumption (like bouyant boussinesqFOam) with the capability to take care of conjugate heat transfer.

What do I get
1. TO test the solver I ran the case of a side heated 2D cavity with
a.) one vertical wall at fixed temperature =300K
b.) one vertical wall with a thickness which undergo conduction and conjugate heat transfer with fluid in cavity
Remaining walls as adiabatic


2. When I run the case in single processor the solution converges and is close to the results from a journal .


What is the issue

When I run it in parallel the solution diverges as the continuity error blows up.

What did I try
1. Tried decomposepar alogrithm Scotch, simple, heirarchial (No useful change)
2.Changes P_rgh solver from PCG to GAMG ...(no useful change)

Could you please suggest anything that I could try with

I tried to reduce the courant number to attain initial stability , but then the solver crashes after 2nd time step.

: Test1
  deltaT = 4.5530327e-107
 Test2  --> FOAM Warning :  From function Time::operator++() in file db/Time/Time.C at line 1061 Increased the timePrecision from 62 to 63 to distinguish between timeNames at time 2.0707573e-07
 Time = 2.07075734119138104400662664383858668770699296146631240844726562e-07   
Solving for fluid region air DILUPBiCG: Solving for T, Initial residual = 0.010403611, Final residual = 2.7324966e-12,
 No Iterations 1 max(T) [0 0 0 1 0 0 0] 300.02011
 DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.0099236724, No Iterations 251 time step continuity errors : sum local = 5.0400286e-07, global = 1.0693134e-19 
-------------------------------------------------------------------------- 
mpirun noticed that process rank 4 with PID 17152 on node n11-42 exited on signal 8 (Floating point exception).

[arjun]

If your calculation diverging in parallel and converging in serial then it is most likely that there is something that is not exchanged properly. 'Properly' is the keyword here, it means that either it is not exchanged or exchanged late enough that when you debug you could be fooled into thinking that all is well when it is not.

[manuc]

Dear Arjun
Thanks for the reply..do u have any suggestions where I should look at in such cases

[arjun]

Originally Posted by manuc

Dear Arjun
Thanks for the reply..do u have any suggestions where I should look at in such cases

It is really difficult to help in this case from outside but I would check what happens with 2 processor run. You should see that it diverges later than other parallel run. If this be the case most probably what i wrote is true.

Now since openfoam is not my area i can not help you much. But i hope others will help you out here.

[manuc]

problem solved:
Temperature anomoly at pressure reference cell