hi

Is there a example/tutorial on how to use the wallHeatFluxIncompe utility?
What should be included in the wallHeatFluxDict?

Thx!

Greetings aevub,

Well... I had already mentioned in my previous post where a "wallHeatFluxDict" can be found:
The package in question that you're probably looking for is in post #12.
This is because the one mentioned on the quoted post is for a modified version of the one in #12.

As for an example case... my guess is that you can use any tutorial case that uses heat transfer and uses incompressible flow.

Best regards,
Bruno

Hello,
i have an other problem with using the wallHeatFluxIncompressible tool. I'm computing a case with the buoyantBoussinesqPimpleFoam in OF 2.2 with k-w SST and wall-functions.
When i'm using the tool it makes the error:

--> FOAM FATAL IO ERROR:
Unknown patchField type kappatJayatillekeWallFunction for patch type wall

Valid patchField types are :
...

Sure i can change the wall function and recompute it but is there a solution with this wall-function?

thanks

Greetings to all!

I've created a git repo for the utility wallHeatFluxIncompressible by Eelco van Vliet: https://github.com/wyldckat/wallHeatFluxIncompressible
In addition, I've adapted the code to work with OpenFOAM 2.2.x and 2.3.x.

Note: When using OpenFOAM 2.2.0, you should use the code that is meant for OpenFOAM 2.1.x, because the field names in 2.2.0 are still using the old field naming convention "kappat" and "kappaEff", while 2.2.1 and above use "alphat" and "alphaEff".


@Chris: I don't know if you've managed to solve the problem you had, but if you're using OpenFOAM 2.2.1 or 2.2.2 or 2.2.x, then try using the code from the repository I've indicated above.

Best regards,
Bruno

Hi all!

I have created a simple model (attached) of natural convection inside a rectangular domain. I used the wallHeatFluxIncompressible utility to check the heat flux balance. I got the expected result, 10 W/m2 were applied to wall4 as BC and 10 W/m2 are coming out wall3 which had a constant temperature BC:

However, in order to get this result I had to set rho0 equal to 1.0 in the transport properties dictionary file (attached).

Could someone explain why this is happenning?

You are working in an incompressible case so pressure is divided by rho. But as I think Openfoam doesn't divide the pressure by your rho, so he uses rho=1 and then

rho0 should be the density of the solver so 1.

This is the only thing I can imagine that can explain it, but I'm pretty sure I'm not right.

Greetings to all!

@kmargaris: From the files in the case you provided, I had to guess that you used the solver buoyantBoussinesqPimpleFoam.

The answer by ssss seems to be correct. More details:

• If you look at the source code for the boundary condition "turbulentHeatFluxTemperature": https://github.com/OpenFOAM/OpenFOAM...hScalarField.C - you'll see this piece of code:
  
  Code:

  ---

          case hsFlux:
        {
            gradient() = q_/(Cp0*alphaEffp);
            break;
        }

  ---

  As you can see, there is no reference to "rho".
• If you look at the respective header file: https://github.com/OpenFOAM/OpenFOAM...hScalarField.H - you'll find this note:
  
  Code:

  ---

  it is assumed that the units of "alphaEff" are [kg/m/s]

  ---

• As ssss indicated, the wallHeatFluxIncompressible utility - https://github.com/wyldckat/wallHeat...compressible.C - uses this equation:
  
  Code:

  ---

  surfaceScalarField heatFlux =fvc::interpolate(alphaEff*Cp0*rho0)*gradT;

  ---

Can you spot the problem?


Essentially, the inverted equation implemented in the boundary condition would be this:
which clearly has no reference to "rho", hence being considered as "1.0".

I took a quick look at the compressible implementation of this boundary condition... and it's essentially the same equation, i.e.:
Which means that some particular detail is being missed here... OK, it looks like the problem is in the units for "alpha":

• incompressible "alphat" field:
  
  Code:

  ---

  dimensions      [0 2 -1 0 0 0 0];

  ---

• compressible "alphat" field:
  
  Code:

  ---

  dimensions      [1 -1 -1 0 0 0 0];

  ---

And there you have it, the reason why "rho" is interpreted as "1.0"... although... the header file "turbulentHeatFluxTemperatureFvPatchScalarFiel d.H" clearly stated that it was assuming "alphaEff" is already in "kg/m/s"... oh my, this looks like a bug in OpenFOAM :eek:! Then again, it's more likely to be a typo in the header's comment!?

So, essentially, the problem is that the heat flux used in the boundary condition is actually "q/rho", i.e. the possibly named kinematic heat flux...


Mmm... I'll report this on the bug tracker...
edit: Bug reported at http://www.openfoam.org/mantisbt/view.php?id=1433

Best regards,
Bruno

@wyldckat: Thanks for the explanation and for submitting the bug report.

It seems that this bug only affects the post processing; the actual heat flux boundary condition is applied correctly in this case, right?

Hi kmargaris,

The boundary condition is incorrect. It would only be correct if Cp0 value was in fact "Cp*rho".
In other words, you can fix the problem for the boundary condition if you simply define "rho" as 1.0 and that "Cp0" is the result of "Cp*rho".

Best regards,
Bruno

Dear wyldckat
 

@ wyldckat

hello, I tried to use your 'wallHeatFluxIncompressible' in my problem. (buoyantBoussinesqPimpleFoam with LES, oneEqEddy)
(I think my result is reasonable when I comparing the temperature and velocity with literature.)
Your utility was completely working and calculating wallHeatFlux!
When I plot the wallHeatFlux, the trend is similar with literature, however, the magnitude is totally different. (e.g. literature: 100, my case: 0.1)

Do you have any idea for this problem?

I use Cp0 =1.005, rho0=1.166

Thank you

Greetings hswzzz,

I'm sorry to say that you haven't provided enough information in order to deduce what might be wrong.

Nonetheless, if I have to guess, since the discrepancy is at a scale of 1000, then my guess is that you were not careful enough with the units of the final mesh. OpenFOAM deals with metre by default and you probably planned for the mesh to be in millimetre.

Best regards,
Bruno

Hi Foamers,

Sorry for restarting the thread again.i am using buoyant boussinesq simpleFoam. i have read most of the threads here how to calculate wall heat flux. now i got a question may be its dumb, I have given temprature b.c on a surface patch is it now possible to find the heat flux on this patch after the simulaion?

i tired the wallheatflux command on the terminal.
can somebody help me.

Thank You.

regards,
Naresh

Hi Bruno,

I also used the turbulentHeatFluxtemperature to specify the heat flux boundary conditions for a patch and i got unphysical result. i m using buoyantboussinesqsimpleFoam. Now i understand the reason. Thanks for the explanation.

That being said is there any other posibility to specify heatFlux boundary condition for a patch?

2. i have another doubt could you please through some light on why should Cp0 should be specified as 1.0. because for TurbulenceHeatFluxTemperature B.C Cp0 is specified as 1006 though they both has the same dimensions m^2/s^2/k

This is very crucial for me right now . thank you.



regards,
Naresh Yathuru

Greetings Naresh,

Installation instructions for compiling wallHeatFluxIncompressible are given here: https://github.com/wyldckat/wallHeatFluxIncompressible

Usage instructions are given in post #19.

This was explained in detail in the posts #27, #29 and in the bug report http://www.openfoam.org/mantisbt/view.php?id=1433

It's not "Cp0" that should be set to "1.0", it's "rho0" that should be "1.0", as already explained in post #29:

Best regards,
Bruno

Hello bruno,

thank you so much for the reply. I have read the posts you have mentioned already. and sorry if my question was not clear. My question was concerning the wallHeatfluxIncompressible. in the readme file it says the following:

Modified version of wallHeatFlux based on suggestion of to change combustion flow to normal flows

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

I replaced the createField with the boussinesqSimpleFoam

In this version it is required to specify values for the density, heat capacity, and Prandtl numbers in the transportProperties dictionary like
could u please through some light on this. i tried but i couldnt figure it out.

may be this is a silly question could you tell me please which value should i use for cp0 and rho0 when i use turbulentwallheatFlux B.C and if i m using the wallheatfluxincompressible utility to find the flux on the patches. should i use Cp0 = 1.0 or 1005.

Thank you,

regards,
Naresh

Hi Naresh,

You'll have to provide more details on how you originally defined your simulation case. Because you're asking about details that relate to post-processing a case I/we know nothing about.
In other words, if you don't indicate how your case was originally created and defined, I don't know how is should be handled at the end of the simulation.

Best regards,
Bruno

thanks for the reply.I am doing a indoor airflow simulation. my geometry is basically a room with inlet, outlet and an object inside.

This is my T B.c

and this how i specified my transport properties
and my 0 folder has wallGradT, wallheatFlux,GradT folders as mentioned in the test case ffor the wallheatFluxincompressible.

when i use turbulentHeatFluxtemperature boundary condition i specify cp0 as 1005. but according to the read me file in the wallheatfluxincompressible it says

My doubt is that, should cp0 be specified as 1.0 or can it be changed according to the case?

i m a little confused.

Thank you
Regards,
Naresh

Hi Eelcovv

Can you please suggest how to use the "wallHeatFluxIncompressible" utilty file. I mean is it like just cope paste the files to the respective directory and than running the utility command from the terminal will work??

Warm regards
Gautam

Hi goutham,


I use it this way. I copy pase the respective files eg, GradT and other required files in the 0 folder before starting the simulation. after the simulation is done u can type wallHeatfluxTemperature and the patchname in yout terminal . it is basically a post processing utility.

i assume u already installed the wallHeatFluxIncompressible utility successfully and checked .

All the best.
Naresh

Hi Naresh

Thanks for your reply. I just downloaded the zipfile given in this thread. After that I am not understanding if to copy the folder to "/applications/utilities" or some other steps to follow. Please help me.

Thanking you
Gautam