[swahono]

Thank you, Maddalena.

I will try it out.

[cbritan]

Originally Posted by maddalena

I commented the if selection while leaving uncommented the inner test in solidWallHeatFluxTemperature.

And where can one find this file? (I too am new to OpenFOAM)

-Clark

[maddalena]

Hi Clark,

Originally Posted by cbritan

And where can one find this file? (I too am new to OpenFOAM)

the original file is this one:
OpenFOAM/OpenFOAM-1.6.x/applications/solvers/heatTransfer/chtMultiRegionFoam/derivedFvPatchFields/solidWallMixedTemperatureCoupled/solidWallMixedTemperatureCoupledFvPatchScalarField .C

Hint: it is always a good idea to create a copy of the original solver to your own folder (OpenFOAM/userID-1.6.x/applications/solvers) before modifying it!

Mad

[maddalena]

Hello everybody,

After a while, I had the chance to work on cht again and, following some suggestions I had, I decided to investigate a little bit deeper the problem of adding an explicit heat source on conduction equation in chtMultiRegionFoam.

Set-up
I created a two solids geometry, similar to what I did here but with region2 larger than before (see geom01.png). I planned 6 different simulations, applying different conditionA and conditionB BC and switching on or off a heat source on region1:

1. Simulation I
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: T = 300K;
   4. Heat source: off;
2. Simulation II
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: coupling;
   4. Heat source: off;
3. Simulation III
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: coupling;
   4. Heat source: on;
4. Simulation IV
   1. time: unsteady;
   2. condition A:symmetry;
   3. condition B: T = 300K;
   4. Heat source: on;
5. Simulation V
   1. time: unsteady;
   2. condition A:symmetry;
   3. condition B: coupling;
   4. Heat source: on;
6. Simulation VI
   1. time: steady;
   2. condition A:symmetry;
   3. condition B: coupling;
   4. Heat source: on;

I selected some points where to sample temperature in time and… well… I let the simulations run… and run… and run… longer and longer than the last time.

Results
What I am more interested in is simulations V and VI, thus the following discussion applies to them. However, similar conclusions can be drawn for the others.

Firstly, I analyzed the temperature variation with position and compared it with theory. Results are reported in xvst.png. As can be seen, results given by steady solver close match the theoretical distribution, while a small error (about 0.5°C) is obtained with the unsteady simulation.

As a second step, I checked time vs temperature for simulation V on the selected point and compare it with the theoretically known temperature variation. As can be seen in figure timevst.png, both using a fixed time step or an adjustable time step, the simulated curves are far to be as in the theory. However, while the fixed time step simulation reaches (almost) the expected steady state temperature for the selected point, the adjustable time step simulation has an unrealistic discontinuity, which spoils the solution before the steady state. Some more tests showed that the position in time of this discontinuity was not affected by the time the solution was saved on the hard disk, but it seems affected by the maxDi value.

Conclusions

• chtMultiRegionFoam and chtMultiRegionSimpleFoam matches the steady state temperature distribution;
• chtMultiRegionFoam is not able to simulate correctly the temperature variation in time;
• chtMultiRegionFoam is not able to reach the steady state solution when using an adjustable time step, but it is when using a fixed time step.

To do
This is for a two solids geometry. What happens when considering a fluid? My next step is to test the same geometry for a steady state & incompressible simulation, with a heat source, using a modified version of this solver.

Notes
is what I reported before these tests wrong? Well, not completely. What I did was to consider the simulation failed when, checking the solution, I could not see the steady state, but this study has showed that chtMultiRegionFoam is not able to simulate correctly the temperature variation in time. Therefore, my error was to consider a total simulation time related to the theoretically known time constant of the solids, while a longer simulated time would have been more appropriate.


Please, can anybody comment on that? Any experience on the subject is welcome, of course!
Regards,

mad

[mirko]

Hi Maddalena,

can you please post archives of setups 5 & 6? I would like to study them some more.

Thank you,

Mirko

[val46]

Hi mad,

I'm also still working on this problem and I think I made some progress. The problem is I have no data from theory to compare my results.
Where do you get this theory data from?
Or do you have any cases for me which I can use for comparison?

Thanks in advance

Toni

[maddalena]

hi guys,
come back in my office today. I will post setup 5 and 6 in the next days, hope within this week. Please, be patient...

mad

[maddalena]

Hi,

@mirko
here are the two cases you asked for. Note that both require a modified model of chtMultiRegionFoam which includes a heat source (variable H). They are ready to run, there is nothing to setup - couple - modify. Hope you find them useful. Please report anything!

@toni
I compared my results with theoretical values you get from formulas for a 1D geometry. Conduction equation, that is it!

Enjoy,

mad

[fisch]

Hello maddalena,

did you finally use "-H" in your TEqun or did you use something like Su(H) for introducing the Volumes?

thanks a lot,
rupert

[maddalena]

Originally Posted by fisch

did you finally use "-H" in your TEqun or did you use something like Su(H) for introducing the Volumes?

-H. That should be fine.

mad

[NicolasB]

Hi Maddalena,

I'd like to study the cooling of a room in which there is a voltage transformer. The heat power is dissipated through a cooling system (seen as a porous medium), with 3 fans behind it. Thanks to your hint I succeeded in setting up the fans' BC.
The question is : is your chtMultiRegionHeatSourceSimpleFoam suited for the job?
If so, would you mind, please, send it at nicolas[dot]bur[at]laposte[dot]net?

Regards

[maddalena]

Just to be clear and for everybody is new here:

Unless what the name says, chtMultiRegionSimpleFoam is for compressible flow: http://foam.sourceforge.net/docs/cpp...674e2e921.html since it implements buoyancy. Let us say that the name SimpleFoam is not really appropriate...

In order to have a steady state, incompressible and turbulent cht solver, one has to modify the solver made by Fabio here: http://www.cfd-online.com/Forums/ope...egionfoam.html. the following should be implemented:

• Make everything independent from temperature.

If an unsteady, incompressible and turbulent solver is required, conjugateHeatFoam (1.6-ext) should be changed. The following should be implemented:

• include more regions: at the moment it supports only one solid one fluid region: http://www.cfd-online.com/Forums/ope...er-region.html
• add turbulence contribution: at the moment it supports only laminar flow.

This is only to trace back my progress (if any... ). Maybe someone else will find them useful. Maybe someone else can tell me if I am wrong.


mad

[andrea.pasquali]

Dear Maddalena,
I'm trying to use chtMultiRegionSimpleFoam (2.1.0) for a Heat Pipe application where I have:
- two incompressible fluids (liquid water and steam) in two different regions
- a solid region whit heat (fuel cell)

I prepared a model with 3 regions (you can see the picture attached).
I resolved "well" (I hope!) problems regarding two phase coupling, incompressiblility, capillarity effects, grid convergence... but what I did not solved yet is the heat flux in "red" patch!
For the heat I used in my "red" BC:
1) temperature fixed value. The simulation reaches convergence but the heat flux I have through the solid region is not enough
2) heat flux fixed value (externalWallHeatFluxTemperature). The simulation doesn't reach convergence. The temperatures rises for ever!
3) fixed gradient. Equal to (2)
4) I tried to use your Vol. Heat Source. I added the field H and changed the solid eqn as:

-fvm::laplacian(kappa, T) - H

But adding Vol. Heat Source what BCs I have to use for H and T? What about the interface between solid and fluid for H?

I'm running now 2 simulation, 1 with zero gradient T and 1 with fixed value T in "red" BC and zero gradient H for both for all solid patches.

I'll report my results here,
Thanks for any help/suggestion

Andrea

[maddalena]

Originally Posted by andrea.pasquali

But adding Vol. Heat Source what BCs I have to use for H and T? What about the interface between solid and fluid for H?

Ciao Andrea,
As for H: I used internalField uniform XXX; and zeroGradient on the boundary patches, including the interfaces between different regions.
As for T: I used internalField uniform ambientTemperature; and zeroGradient or solidWallMixedTemperatureCoupled on the boundary patches, depending if the coupling was needed or not.
Hope this help,
mad

[andrea.pasquali]

Hi,
here my (first) results with Vol. Heat Source in solid region and:
1) T fixedValue at "red" patch
2) T zeroGradient at "red" patch
As you can see from pictures:
1) with fixedValue (T_fV.jpg) the temperatures seem to reach convergence but the T at interface steam/solid is grater than the free solid wall ! This is very strange for me because the heat is going out the domain (?)...
2) with zeroGradient (T_zG.jpg) the temperatures don't seem to reach convergence... or how many iterations I need to?

Now it seems that using Vol. Heat Source in solid region instead heat flux in "red" patch does not solve the problem.... the T doesn't converge too.

My question is: how is the correct way to set Heat Flux? (I have already tried fixedGradient, externalWallHeatFluxTemperature, vol. heat source...).
It seems only T fixed value allow me to reach convergence, but T fixed value at "red" patch is not what I want!
Maybe steady state is not good for this? Do I need transient?

Any comment is useful!

Thanks

Andrea

[sitekss]

Dear Foamers,
I'm playing with chtMultiRegionFoam, in my case I would like to have heat source too. I added:

"-H" to solveSolid.H,

" volScalarField H (
IOobject
(
"H"
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
),
mesh
);" to setRegionsSolidField.H
and
"PrtList<volScalarField> H(solidRegions.size());" to createSolidFields.H


I can compile my solver but it returns error:
Cannot find file
file /.../cht/0.0588235/solid/H
Where is the problem? It seems that the solver can't read 0/H file.

[FabienF]

Hi Maddalena,
I am working on the same implementation and I am facing the same problem. Did you make any progress on this issue?
Fab

[ahmmedshakil]

Hi Maddalena,
Can you please advice me how added the volume heat source to the chtMultiregionFoam ? My problem is similar to yours (heat transfer between to different solids).
Thanks in advance.
shakil

Originally Posted by maddalena

Hello everybody,

After a while, I had the chance to work on cht again and, following some suggestions I had, I decided to investigate a little bit deeper the problem of adding an explicit heat source on conduction equation in chtMultiRegionFoam.

Set-up
I created a two solids geometry, similar to what I did here but with region2 larger than before (see geom01.png). I planned 6 different simulations, applying different conditionA and conditionB BC and switching on or off a heat source on region1:

1. Simulation I
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: T = 300K;
   4. Heat source: off;
2. Simulation II
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: coupling;
   4. Heat source: off;
3. Simulation III
   1. time: unsteady;
   2. condition A:T = 350K;
   3. condition B: coupling;
   4. Heat source: on;
4. Simulation IV
   1. time: unsteady;
   2. condition A:symmetry;
   3. condition B: T = 300K;
   4. Heat source: on;
5. Simulation V
   1. time: unsteady;
   2. condition A:symmetry;
   3. condition B: coupling;
   4. Heat source: on;
6. Simulation VI
   1. time: steady;
   2. condition A:symmetry;
   3. condition B: coupling;
   4. Heat source: on;

I selected some points where to sample temperature in time and… well… I let the simulations run… and run… and run… longer and longer than the last time.

Results
What I am more interested in is simulations V and VI, thus the following discussion applies to them. However, similar conclusions can be drawn for the others.

Firstly, I analyzed the temperature variation with position and compared it with theory. Results are reported in xvst.png. As can be seen, results given by steady solver close match the theoretical distribution, while a small error (about 0.5°C) is obtained with the unsteady simulation.

As a second step, I checked time vs temperature for simulation V on the selected point and compare it with the theoretically known temperature variation. As can be seen in figure timevst.png, both using a fixed time step or an adjustable time step, the simulated curves are far to be as in the theory. However, while the fixed time step simulation reaches (almost) the expected steady state temperature for the selected point, the adjustable time step simulation has an unrealistic discontinuity, which spoils the solution before the steady state. Some more tests showed that the position in time of this discontinuity was not affected by the time the solution was saved on the hard disk, but it seems affected by the maxDi value.

Conclusions

• chtMultiRegionFoam and chtMultiRegionSimpleFoam matches the steady state temperature distribution;
• chtMultiRegionFoam is not able to simulate correctly the temperature variation in time;
• chtMultiRegionFoam is not able to reach the steady state solution when using an adjustable time step, but it is when using a fixed time step.

To do
This is for a two solids geometry. What happens when considering a fluid? My next step is to test the same geometry for a steady state & incompressible simulation, with a heat source, using a modified version of this solver.

Notes
is what I reported before these tests wrong? Well, not completely. What I did was to consider the simulation failed when, checking the solution, I could not see the steady state, but this study has showed that chtMultiRegionFoam is not able to simulate correctly the temperature variation in time. Therefore, my error was to consider a total simulation time related to the theoretically known time constant of the solids, while a longer simulated time would have been more appropriate.


Please, can anybody comment on that? Any experience on the subject is welcome, of course!
Regards,

mad

[ageorg]

Dear All,

I am solving a multisolid domain consisting of three different solids one in the bottom, one in the middle and one in the top.
I apply a fixed temp Gradient at the bottom patch of the bottom solid which is the heat flux (W/m2) divided by the thermal conductivity (k) of the bottom solid (W/mK). When i use the same k for all three solids the results are as expected. However when i use a different k for the middle solid the results are not correct.

Can anybody help me

Thanks

T.

[bibin.sme]

could you please give me some idea how to add a porous media in chtMultiRegionFoam.
I wanted to model Heat pipe in openFoam. For the same I created a duct in Gambit ( please see the attached image file).

In gambit I created 3 regions as shown in figure. now the problem I'm facing is how to specify the boundary conditions for the field variables at the interfaces for U, T, p_rgh.

could u please tell me how to add source terms for 3 regions to in-cooperate both heat transfer & porosity.

Regards,
Bibin