The temperature values are still blowing up.
 

Hello there.


This is a continuation thread from {https://www.cfd-online.com/Forums/openfoam/203614-chtmultiregionfoam-source-core-defined-field-e-but-never-used.html#post698295} I started it because this post is off-beat from the previous post.



I am using a chtMultiRegionSimpleFoam solver to simulate the flow over a hot prismatic cell kept inside air flow region.



The block has a heat source of 7W, has dimension: 210*135*30mm^3



At t=0:


Air temperature: 300 K
Block temperature: 310 K


Inlet Air velocity: 0.5 m/s


The solver runs finely but there is a huge problem in the block temperature.

I can see in the log file (cant attach it here due to the permissible upload limits. Screenshot is attached.) that the block temperature reaches upto 930 K. I cant possibly imagine how is that possible? Since a rough calculation on paper gives me a maximum temperature of 314 K for the block.


Can anyone please reflect back on this problem? It will be a huge help.

I think i have got the error.

In the .stl files of geometry, i had incorrectly scaled everything by the factor of 0.1. Now the error is rectified, and the temperature values are realizable.

Will keep you updated regarding the final results.


Regards.
Rajat

Hello,

The simulation has in my opinion the right setup.

Which dimensions has the block?

I am measuring block = 3 X 22 X 13.5 mm³

is that right?

Regards

Peter

PS: OK you were faster with your post :)

how can i put in thermal conductivity as different for x,y,z for my block?


currently: K = 235


What I want: K = (0.983 38.54 38.54)



Please refer to the attached pic


Regards,
Rajat

I was running the case for different set of inlet velocity of air.

Somehow, a huge inconsistency has popped up.



Using your test case setup, for the same set of inlet conditions i am getting two different type of temperature variation for two cases. Sorry if that confuses you; it is confusing indeed.



Test case1: The max Temp value mentioned in log file at iteration 1 is 300.0093 K



Test case2: The max Temp value mentioned in log file at iteration 1 is 321.0166 K



I have attached the screenshots of the log file since the file itself is superheavy.



It will be a great help if you can explain this discrepancy.


Regards,
Rajat

Well the two cases seams to have identical inlets of 0.5 for both cases.

All boundaries and setups seams to be identical.

Except the relaxationsFactor of h for the block!

In the case 1 the relaxationsFactor is 0.7.

In the case 2 the relaxationsFactor is 1.0.

That is why the progress in the temperatur increasing for the block in the first case much slower than the second.

It is an experience factor how to define the relaxationsfactor.

it is recommended for such a case to be 1 for h for the solid regions.

Just if the calculation become unstable then you can reduce it.

The relaxationFactor as defined in the second case are good defined because you reach the results fast and stable!

Both cases brings the same results.

Anyway, the case 1 needs more iterations!

Regards

Peter

Thanks a lot.

One more thing i needed to ask is about the residuals [Pic attached]. First they decrease, then increase a little and then become constant for a while.

Although my learning curve right now is super-steep, i think for a good convergence residuals should continuously decrease, right?

The problem is just to be recognized for big geometries.

For small geometries I could not find any problem.

Example was cht_cas_Works I uploaded earlier. It works very fine.

The same simulation makes problem when scaling 10 times bigger.

Very interesting phenomena :)

I berlive that the problem could be solved by activating the turbulance.

I will give feedback when testing finisch!

Regards

Peter

Hi,


I would like to ask a little thing.



I was trying to add the k-omegaSST turbulence model, so tried to copy/paste the fvSolution and fvSchemes files from a default tutorial (like buoyantCavity) in which this model has been used. But since fvSolution and fvSchemes are separately defined for air and block, how should i copy them exactly?



And also are there any other files which need to be changed?


I have referred this tutorial: {http://www.mmm.ulg.ac.be/files/MECA0025/Projet/From_laminar_to_turbulent.pdf}



regards,


Rajat

Hi,

I did not use k-omegaSST before.

I cant say exactly what to use!

Anyway as a general rule, always try to use what already works and then try something new.

https://www.openfoam.com/documentati...a-sst-des.html

In the tutorials under:

../tutorials/heatTransfer/chtMultiRegionSimpleFoam/heatExchanger/

There is a turbulence model used.

Copy the files from here and then optimize or modefy them for your needs.

To be copied/modified:

-system:

fvSolution

fvShemes

Modify changeDictionaryDict (by adding the changes for turbulence).

- constant/{Fluid}:

Activating turbulence and defining turbulence parameters in turbulenceProperties

- 0:

Adding the turbulence initial conditions for the fluids


Anyway, try to play with the existing tutorials first before going forward :)

Regards

Peter

Hi Peter,


Meanwhile trying out the turbulence model, I also did some post-processing of the previous results.



In Paraview, i find it hard to draw contour plots for my results. I have attached a picture to show you exactly what kind of plots i need.



While using the contour filter in paraview, i get isosurfaces. But thats not what i am looking for. If you can suggest a tutorial then it would be great.



Or just any other software to do so.


Regards,


Rajat