CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Post-Processing

How to calculate heat flow from wall to the surrounding environment in of 2.1.1

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 18, 2014, 02:27
Default How to calculate heat flow from wall to the surrounding environment in of 2.1.1
  #1
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Greeting All,
I am trying to solve a case in chtMultiRegionSimpleFoam for a geometry of cavity is surrounded by some thickness of insulation.

My question is how to calculate the heat flow from outside of insulating wall to the environment in openfoam 2.1.1.....

Please sugeest how should I do this thing? I have gone through some threads in CFD forum but can't get properly.....

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 18, 2014, 12:42
Default
  #2
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
Hi Baran,

I think what you need is wallHeatFlux utility. This is a post processing tool that computes the heat flux across all boundaries of your geometry. These boundaries need to be specified as wall, if they are previously specified as patch instead I think wallHeatFlux won't compute any flux across them.

Hope it helps!


Regards,

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 19, 2014, 00:11
Default
  #3
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
@ alex ....thanks fro your suggestion....
I tried with
Quote:
wallHeatFlux
postProcessing utility.....it is working...for fluid region properly.....
but for solid region it is not working....
for my case I want to calculate how much heat is flowing from solid wall to environment....which is having mixed boundary condition of h & Tamb.....

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 19, 2014, 16:09
Default
  #4
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
Have you tried the -region flag? If boundaries have been defined as wall it must work.

Regards

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 21, 2014, 23:02
Default
  #5
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Greeting all,

@alex ..I tried with this command but it is searching for file..
Quote:
thermophysicalProperties
and showing fatal error.......
...it is not reading.....

Quote:
solidThermoPhysicalProperties
for solid region...

please suggest something.......

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 22, 2014, 00:52
Default
  #6
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Hello all,
I just went through solver of the utility...wallHeatFlux...and it is meant for fluid region...
Quote:
surfaceScalarField heatFlux
(
fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h)
);
Can you suggest how to give heat flux.....command for...solid region....

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 22, 2014, 01:58
Default
  #7
New Member
 
Join Date: Mar 2014
Posts: 8
Rep Power: 4
karoltomek is on a distinguished road
I am using chtMultiRegionSimpleFoam solver (OF 2.3 and 2.2) and wallHeatFlux utility works for me. Do you have all needed files?
In fluid region directory I have:
- g
- RASProperties
- thermophysicalProperties
- turbulenceProperties
In solid region directory I have:
- radiationProperties
- thermophysicalProperties

And look at my fvSchemes settings file for solid region:

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
}

laplacianSchemes
{
default none;
laplacian(alpha,h) Gauss linear uncorrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default uncorrected;
}

fluxRequired
{
default no;
}
karoltomek is offline   Reply With Quote

Old   September 22, 2014, 02:13
Default
  #8
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Hello,
I am using OF 2.1...here for solid region file name is ..
Quote:
solidThermoPhysicalProperties
this wallHeatFlux utility is unable to read this file for solid region....

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 22, 2014, 13:21
Default
  #9
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
Are you sure that the file is called solidThermoPhysicalProperties instead of simply thermophysicalProperties??

I have never worked with OF 2.1.1 but i have tried OF 2.2.1 and 2.3.x and the file name in these versions is the second one.

Can you post the whole message given out by OF so that it could be easier for the experts (not me) to find the problem?


Regards,

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 23, 2014, 04:20
Default
  #10
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Quote:
[bg8743@INDUX08 wallHeatFlux_consT]$ wallHeatFlux
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.1-221db2718bbb
Exec : wallHeatFlux
Date : Sep 23 2014
Time : 13:37:19
Host : "INDUX08.in.com"
PID : 24470
Case : /home/bg8743/OpenFoam/tutorials/heatTransfer/chtMultiRegionSimpleFoam/wallHeatFlux_consT
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0


--> FOAM FATAL IO ERROR:
cannot find file

file: /home/bg8743/OpenFoam/tutorials/heatTransfer/chtMultiRegionSimpleFoam/wallHeatFlux_consT/constant/thermophysicalProperties at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

[bg8743@INDUX08 wallHeatFlux_consT]$

may be solid region is not included for wallHeatFlux utility....
please suggest how to modify this for solid region....
baran_foam is offline   Reply With Quote

Old   September 23, 2014, 05:45
Default
  #11
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
The problem is that the file is being searched within the constant folder instead of the constant/solidRegion folder. Besides that you are executing wallHeatFlux instead of WallHeatFlux -region solidRegion.

Regards,

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 23, 2014, 06:57
Default
  #12
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Greeting all,

@Alex....in my case i am unaware oe the command...given by you..so I make a folder of each region separately to check the wall heat flux......
by the command ..
Quote:
wallHeatFlux -region <NAME>
same error is showing.........

for further study...I name this solidThermophysicalProperties as thermophysicalProperties.....so i got this kind of comment.....

Quote:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0
Selecting thermodynamics package constSolidThermo


--> FOAM FATAL ERROR:
Unknown basicThermo type constSolidThermo

Valid basicThermo types are:

26
(
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<incompressible>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<icoPoly3ThermoPhysics>>
hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<constTransport<specieTherm o<hConstThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
)



From function basicThermo::New(const fvMesh&)
in file basicThermo/basicThermoNew.C at line 60.

FOAM exiting

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 23, 2014, 07:26
Default
  #13
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
Have you defined properly both solid and fluid regions in the "constant/regionProperties" file?
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 23, 2014, 07:31
Default
  #14
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
@ alex...I hope I defined this properly......
but it is not built for solid region.......

Regards,
baran
baran_foam is offline   Reply With Quote

Old   September 23, 2014, 07:40
Default
  #15
Senior Member
 
Alex
Join Date: Oct 2013
Posts: 332
Rep Power: 14
zfaraday will become famous soon enough
Then I don't know what the problem can be... Maybe if you upload your case someone could check it out in order to help you.

Regards and cheer up!

Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com

The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!
zfaraday is offline   Reply With Quote

Old   September 25, 2014, 04:25
Default wallHeatFlux utility for solid region in OF 2.1.1
  #16
Member
 
baran
Join Date: Aug 2014
Posts: 45
Rep Power: 4
baran_foam is on a distinguished road
Greeting all,
In this way i have modified wallHeatFlux utility...for OF 2.1.1 ...now it working properly.....
In createField.H
Code:
autoPtr<basicSolidThermo> thermo
(
basicSolidThermo::New(mesh)
);
const volScalarField& T = thermo->T();
tmp<volScalarField> tkappa = thermo->K();
//tmp<volSymmTensorField> tkappa = thermo.directionalkappa();
const volScalarField& kappa = tkappa();
In wallHeatFlux.C ..
Code:
surfaceScalarField heatFlux
(
fvc::interpolate(kappa)*fvc::snGrad(T)
);
In Make/option
Code:
EXE_INC = \
    -I$(LIB_SRC)/turbulenceModels \
    -I$(LIB_SRC)/turbulenceModels/compressible/RAS/RASModel \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basicSolidThermo/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = \
    -lcompressibleRASModels \
    -lfiniteVolume \
    -lgenericPatchFields \
    -lspecie \
    -lbasicSolidThermo
Now it working properly...may be useful for some oher foamer...

Regards,
baran

Last edited by wyldckat; September 28, 2014 at 11:41. Reason: Changed [QUOTE][/QUOTE] to [CODE][/CODE]
baran_foam 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
CFX fails to calculate a diffuser pipe flow shenying0710 CFX 7 March 26, 2013 05:13
Heat Transfer Coefficient in Compressible Flow 3D turbine cascade Karkoura CFX 0 March 10, 2011 16:35
Flow around pipes - heat transfer coefficient on the wall of pipe doodek Main CFD Forum 2 November 23, 2009 09:48
No results for solid domain Gary Holland CFX 10 March 13, 2009 04:30
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02


All times are GMT -4. The time now is 02:38.