CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Fixed heat flux BC in buoyantPimpleFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree18Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 30, 2011, 03:45
Default
  #21
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 9
mabinty is on a distinguished road
Quote:
Originally Posted by murrdpirate View Post
Thanks. I didn't realize there were examples in the code for these things.

Issue now is that it's saying "KName is undefined." As you showed, that's not listed in the example. I see somewhere online that it's "CHARACTER*(*) array of species names," but I don't know what that means
It would be easier to figure out the problem if we can see the exact error message! Try to add the line:

Code:
KName          K;
Check src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/temperatureCoupledBase/temperatureCoupledBase.C to see what is happening with "KName".

Cheers,
Aram
murrdpirate likes this.

Last edited by mabinty; June 30, 2011 at 03:46. Reason: typo
mabinty is offline   Reply With Quote

Old   June 30, 2011, 17:53
Default
  #22
Member
 
Kevin
Join Date: May 2011
Posts: 32
Rep Power: 7
murrdpirate is on a distinguished road
Here's the error I get when KName isn't defined:

Quote:
--> FOAM FATAL IO ERROR:
keyword KName is undefined in dictionary "/home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0/T::boundaryField::window"

file: /home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0/T::boundaryField::window from line 44 to line 49.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 400.

FOAM exiting

Your suggestion to add "KName K;" made sense and actually did allow my case to calculate as normal, but for some reason I get the following error when I try to view the data in paraView (I also get the same error when running reconstructPar if I calculated in parallel):


Quote:
--> FOAM FATAL IO ERROR:

Cannot find 'value' entry on patch walls of field T in file "/home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0.0005/T"
which is required to set the values of the generic patch field.
(Actual type compressible::turbulentHeatFluxTemperature)

Please add the 'value' entry to the write function of the user-defined boundary-condition


file: /home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0.0005/T::boundaryField::walls from line 77556 to line 83919.

From function genericFvPatchField<Type>::genericFvPatchField(con st fvPatch&, const Field<Type>&, const dictionary&)
in file genericFvPatchField/genericFvPatchField.C at line 71.

FOAM exiting
Again, thanks for the help, I do feel like I'm at least getting there. I'll look into this a little bit more tonight when I have time and share what I find.
murrdpirate is offline   Reply With Quote

Old   June 30, 2011, 23:21
Default
  #23
New Member
 
Mark Pitman
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 7
Rep Power: 9
pitmanm is on a distinguished road
I can confirm that this error occurs also when attempting to recomposePar a model that makes use of turbulentHeatFluxTemperature boundary condition.

It appears to be a bug in the turbulentHeatFluxTemperature boundary condition in OpenFOAM 2.0 where this BC does not write the "value" entry for this BC. A look at the code seems to confirm this.

I am thinking of copying the BC to create a user-defined boundary condition which fixes the problem of writing the 'value' entry. Does anyone else know of a fix or workaround that I may not have considered?
pitmanm is offline   Reply With Quote

Old   July 7, 2011, 07:18
Cool
  #24
New Member
 
Mauro Arruda
Join Date: Oct 2010
Posts: 1
Rep Power: 0
mauro.p.arruda@gmail.com is on a distinguished road
hi pitmanm,

have you been able to get around the bug?

Get the same problem when converting the time directories for post-processing.

I just started looking into it and will let you know if i'm lucky or not

Cheers,

Mauro
mauro.p.arruda@gmail.com is offline   Reply With Quote

Old   July 7, 2011, 13:24
Default
  #25
New Member
 
Mark Pitman
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 7
Rep Power: 9
pitmanm is on a distinguished road
Hi Mauro,

I have not had a chance as of yet because I've been so busy with work. The change in the code is pretty easy it is just actually just getting the fvPatchScalarField to work as a user-defined BC I have found tricky. Do you need to do it all as template classes? Then just define <scalar> perhaps?

Cheers,

Mark
pitmanm is offline   Reply With Quote

Old   September 2, 2011, 07:52
Default
  #26
New Member
 
Maria Jaromin
Join Date: Sep 2011
Posts: 2
Rep Power: 0
jaromin is on a distinguished road
Hi,

"The problem is that the postprocessing utilities do not know about that b.c. so do not know how to read it (it is derived from a fixedGradient b.c. which does not need a 'value' field).

If you add the library that contains the compressible::turbulentHeatFluxTemperature to your 'libs' section in the system/controlDict it should work.

libs ("libcompressibleTurbulenceModel.so"); "

see: http://www.openfoam.com/mantisbt/view.php?id=285

Maria
bhh likes this.
jaromin is offline   Reply With Quote

Old   September 19, 2012, 12:33
Default
  #27
New Member
 
anonymous
Join Date: Sep 2012
Location: Miami, USA
Posts: 7
Rep Power: 5
socrates is on a distinguished road
I am trying to apply a constant BC on micro-tubes surfaces inside a substrate. I have tried these:
1.

{
type fixedGradient;
gradient uniform -10000;
}

2.

{
type groovyBC;
gradientExpression "-10000";
fractionExpression "0";
}

3.

{
type groovyBC;
value uniform 300;
gradientExpression "gradT";
variables "htot=15000.00;Tinf=293.00;k=130;gradT=htot/(k)*(Tinf-T);";
}

The results show different gradient values on the walls, gradTx, gradTy and gradTz are so much more that the input values. I should mention that when I apply this BC for top surface which is horizontal I get perfect results. Here it says ( http://www.foamcfd.org/Nabla/guides/...Guidese11.html) that by "fixedgradient" we define
. I need to define only the magnitude of temperature gradient on the tubes.

Could you help me please?

Thank you

aa
socrates is offline   Reply With Quote

Old   September 21, 2012, 02:48
Default
  #28
New Member
 
Matthias Hettel
Join Date: Apr 2011
Location: Karlsruhe, Germany
Posts: 28
Rep Power: 7
matthi is on a distinguished road
Hello Socrates,

I don`t understand your physical problem and why you need a fixed gradient. May be you could also use a fixed heat flux?
Nevertheless, I have some experience in defining boundary conditions for solid regions. Maybe, you find something useful in the solver:

OpenFOAM-1.7.\applications\solvers\heatTransfer\chtMultiReg ionSimpleFoam

The boundary conditions can be find in the subfolder

derivedFvPatchFields\solidWallHeatFluxTemperature

Good luck

Matthi
matthi is offline   Reply With Quote

Old   May 30, 2013, 22:21
Default
  #29
Member
 
George Pichurov
Join Date: Jul 2010
Posts: 39
Rep Power: 8
jorkolino is on a distinguished road
Quote:
Originally Posted by mabinty View Post
That means you did not specify how the conductivity fied "K" shoud be calculated. Look at the top of src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.H:

Code:
hotWall
        {
            type            compressible::turbulentHeatFluxTemperature;
            heatSource      flux;        // power [W]; flux [W/m2]
            q               uniform 10;  // heat power or flux
            K               basicThermo; // calculate K by alphaEff*thermo.Cp
            value           uniform 300; // initial temperature value
        }
Cheers,
Aram
In my case, the error message says keyword alphaEff is undefined. Shall I use the same assignment as for the K keyword above? Forgot to mention, my solver buoyantBoussinesqSimpleFoam. Nope, it does not work, I tried define the alphaEff keyword as above, but it is rejected as a valid entry in the basicThermo.

Last edited by jorkolino; May 31, 2013 at 01:15. Reason: Add details
jorkolino is offline   Reply With Quote

Old   January 29, 2015, 02:49
Default please suggest how to solve this error
  #30
New Member
 
Rahul
Join Date: Jan 2015
Posts: 1
Rep Power: 0
rahulps is on a distinguished road
--> FOAM FATAL IO ERROR:
keyword kappa is undefined in dictionary "/home/rahulps/OpenFOAM/rahulps-2.2.2/run/conjugate1/0/solid/T.boundaryField.solid_to_fluid"

file: /home/rahulps/OpenFOAM/rahulps-2.2.2/run/conjugate1/0/solid/T.boundaryField.solid_to_fluid from line 41 to line 45.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 402.

FOAM exitin
rahulps is offline   Reply With Quote

Old   March 10, 2015, 10:21
Unhappy error: keyword alphaEff is undefined in dictionary
  #31
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 55
Rep Power: 3
Naresh yathuru is on a distinguished road
Hi Foamers,

I m using openFoam 2.3.0 and the solver is buoyantBoussinesqsimpleFoam. I am simulating a room with a cube inside i have to impose heat flux boundary conditions..Therefore i applied turbulentHeatFluxTemperature bc for the patch as follows
innercube
{
type turbulentHeatFluxTemperature;
heatSource flux; //power;
q uniform 100;
value uniform 293.0;
}

Now i m getting a error as innercube

keyword alphaEff is undefined in dictionary "/home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube"
[7]
[7] file: /home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube from line 40 to line 43.
[7]
[7] From function dictionary::lookupEntry(const word&, bool, bool) const
[7] in file db/dictionary/dictionary.C at line 437.
[7]
FOAM parallel run exiting

I have read in the forum that i should change kappaeff to alphaeff in th Tequ.H but it turns out the new version already has the changes implimented. so i m not sure where i m went wrong.
could someone please help help me. im desperate for help.
Naresh yathuru is offline   Reply With Quote

Old   March 10, 2015, 10:23
Default
  #32
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 55
Rep Power: 3
Naresh yathuru is on a distinguished road
Hi rahul and george

i have a similar error how did u alble to solve your error coul you please help me.

Thankyou

regards,
Naresh
Naresh yathuru is offline   Reply With Quote

Old   March 11, 2015, 04:47
Default
  #33
Senior Member
 
AgustÝn Villa
Join Date: Apr 2013
Location: Brussels
Posts: 103
Rep Power: 5
agustinvo is on a distinguished road
Quote:
Originally Posted by Naresh yathuru View Post
Hi Foamers,

I m using openFoam 2.3.0 and the solver is buoyantBoussinesqsimpleFoam. I am simulating a room with a cube inside i have to impose heat flux boundary conditions..Therefore i applied turbulentHeatFluxTemperature bc for the patch as follows
innercube
{
type turbulentHeatFluxTemperature;
heatSource flux; //power;
q uniform 100;
alphaEff alphaEff;
value uniform 293.0;
}

Now i m getting a error as innercube

keyword alphaEff is undefined in dictionary "/home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube"
[7]
[7] file: /home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube from line 40 to line 43.
[7]
[7] From function dictionary::lookupEntry(const word&, bool, bool) const
[7] in file db/dictionary/dictionary.C at line 437.
[7]
FOAM parallel run exiting

I have read in the forum that i should change kappaeff to alphaeff in th Tequ.H but it turns out the new version already has the changes implimented. so i m not sure where i m went wrong.
could someone please help help me. im desperate for help.
Hello

You have to declare inside your BC which variable would be your alphaEff. Otherwise the BC code cannot continue.

In relation with the name of the variable, it does not matter if you have defined it in the solver. So you could put
Quote:
alphaEff alphaEff;
or
Quote:
alphaEff kappaEff;
agustinvo is offline   Reply With Quote

Old   March 11, 2015, 06:27
Default
  #34
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 55
Rep Power: 3
Naresh yathuru is on a distinguished road
Hi augstin villa and other Foamers,

Thanks for your reply.

It took me a some time to find it out and itseems nobody left any trace of the changes in new version but i m glad to share this. In openFoam version 2.3.0 the thermal diffusivity kappaeff in turbulence heatflux temperature is already replacded to alphaeff.

And aditionally u have to include Cp0 Cp0 1005 in the ttransport properties. Note (no dimention for Cp0)

Fore more details check turbulenceheatfluxtemperature.H

hope this would help people like me who arre new to openFoam

Regards,
Naresh
agustinvo likes this.
Naresh yathuru is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Sign of Heat Flux at wall Kyung FLUENT 2 February 26, 2016 17:25
Variable name for heat flux peterle CFX 4 February 13, 2014 03:21
Heat Flux Wall Boundary Confusion. Joee FLUENT 1 August 21, 2010 12:20
Heat flux in ansys cfx juliom OpenFOAM Running, Solving & CFD 2 April 14, 2009 14:30
Total heat transf. rate vs Total surface heat flux Renato Sousa FLUENT 0 August 22, 2005 10:34


All times are GMT -4. The time now is 04:16.