CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   heat transfer with RANS wall function, over a flat plate (validation with fluent) (http://www.cfd-online.com/Forums/openfoam-solving/100352-heat-transfer-rans-wall-function-over-flat-plate-validation-fluent.html)

 bruce April 24, 2012 10:29

heat transfer with RANS wall function, over a flat plate (validation with fluent)

Hi all,

I am following this test case,(forced convection over a flat plate)
https://confluence.cornell.edu/displ...+Specification

OpenFOAM vs (Fluent & Theory & Experiment)

It is a compressible, RANS, low-Re grid with realizable k-epsilon model. The above link matches that fluent , theory , experiment results in agreement.

My aim is to prove the same from OpenFOAM side.

I use 2.1.x (latest git) rhoSimpleFOAM solver, realizableKE (RANS turbulence model !)

So i try to use same settings as in fluent above.

Test 1: laminar
The heat transfer values at the plate are in agreement with fluent. I have used (wallHeatFlux -latestTime) the standard utility

Test 2: with turbulence model
The heat transfer values are quite different :eek: !! My doubt is either the realizableKE model or wall functions.

U: mutkWallFunction
k: compressible::kqRWallFunction
epsilon: compressible:epsilonWallFunction
alphat: alphatJayatillekeWallFunction

Since the pressure variations are very small, it is not a good idea to work with abs. pressure field , so i modified thermophysical models and recompiled rhoSimpleFoam solver. Now that, i have guage pressure formulation for pressure !!!

Now i do not know why i get different wall heat flux value on the plate when compare to fluent (of course, fluent results are in agreement with experiment and theory as i said above)

inside rhoSimpleFoam: run ./Allwmake

if you need laminar test case , let me know.

The heat flux value from fluent and OpenFOAM (in case you do not have fluent)

Code:

```#position Fluent OpenFOAM 0.0166667  322.544 284.76711 0.05    220.942 85.636212 0.0833333  200.35  62.086357 0.116667    188.401 52.34236 0.15    179.175 46.641522 0.183333    171.331 42.556804 0.216667    164.508 39.520929 0.25    158.538 37.0035 0.283333    153.292 35.036207 0.316667    148.668 33.252812 0.35    144.577 31.856434 0.383333    140.945 30.491744 0.416667    137.708 29.45537 0.45    134.812 28.357696 0.483333    132.213 27.569636 0.516667    129.872 26.652224 0.55    127.754 26.048582 0.583333    125.833 25.257404 0.616667    124.084 24.79662 0.65    122.486 24.094795 0.683333    121.021 23.750895 0.716667    119.673 23.112447 0.75    118.428 22.866211 0.783333    117.276 22.272958 0.816667    116.202 22.109839 0.85    115.206 21.549314 0.883333    114.267 21.455807 0.916667    113.377 20.919178 0.95    112.623 20.88645 0.983333    111.442 20.361769```
(If you need fluent files, let me know)

If someone is curious to validate OpenFOAM Wall function here, Link for OpenFOAM test case,
http://cdn.anonfiles.com/1335277397283.zip

Thanks

 DAOU M.P. May 2, 2012 04:56

Hi,
I observe the same differences for the heat flux value between fluent and OpenFOAM for this test case.
I use buoyantSimpleFoam solver, realizableKE.
I don't understand these differences.
If someone has an idea of ​​the reason for these differences?
I think if the can come from the difference of calculated heat flow.
I calculate the heat flux: k * magGradT and magGradT is calculated with "foamCalc magGrad T"
And I compare in Fluent with Total Surface Heat Flux but I don't sure that it is equivalent.
Best regard,

 bruce May 4, 2012 14:44

Hi,

In order to simplify my case, i created blockMesh coarse grid with yPlus (or yStar) from 16 to 23. And have changed turbulence model to standard k-epsilon instead of realizableKE.

I have results from fluent with standard k-epsilon with standard wall function so that i would verify this in OpenFOAM. Unfortunately, it is still not comparable. I feel that there could be a bug some where.

I used rhoSimpleFoam although buoyancy solver can also be used, it is the same for our case.

Heat flux in OpenFOAM is: qDot = alphaEff| v-> f * grad(h) but i am not sure about fluent.

here is the complete case set:

http://cdn.anonfiles.com/1336156429443.zip

Upon generating results which is comparable to fluent, one can say that OpenFOAM wall functions are working as so.

Thanks

 fredo490 April 17, 2013 10:10

Hello,
Did you succeed to get accurate results ? Did you find any improvement ?

Thx, Fred

 PainInTheMesh September 24, 2013 20:12

I cannot run either for some reason - I am trying to find a validation case where heat transfer is solved to the walls, utilizes a wall function, and is internal flow. Does anyone know of any cases that can be validated?

 bruce September 25, 2013 04:40

Hi,

as far as i remember, my test case is correct. OpenFOAM and Fluent gave well comparable results. The problem was in my side while calculating heat flux. The values posted also correct.

May be it will help you to further expriment with.

Rgds,

 All times are GMT -4. The time now is 21:36.