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

Heat transfer with solid elements conduction

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 16, 2006, 04:42
Default I found the error.. it was a s
  #61
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
I found the error.. it was a stupid mistake in the evaluation of the heat conductivity ratio..

I attach the modified version for people interested..

Daniele

conjugateFoam7.tar.gz
panara is offline   Reply With Quote

Old   February 16, 2006, 05:36
Default Hi, Daniele, Thank you for
  #62
New Member
 
Masato Otsuki
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 26
Rep Power: 8
otsuki is on a distinguished road
Hi, Daniele,

Thank you for uploading interesting solver and case.
In my OpenFoam-1.2 distribution, your solver cannot
be built by wmake.
In your Make/options,

EXE_INC = \
-I$(LIB_SRC)/cfdTools/compressible \
-I$(LIB_SRC)/cfdTools/lnInclude \
...

But my system, there is no lnInclude/
in cfdTools/ directry but exist in
cfdTools/general/

The version of OpenFOAM is different with yours ?


Masato Otsuki
otsuki is offline   Reply With Quote

Old   February 16, 2006, 12:41
Default You are right, I should have m
  #63
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
You are right, I should have mentioned that I am using the 1.1 version of OpenFoam...

If you change cfdTools with cfdTools/general it should work.

You have also to change the Peqn.H file according to the 2.2 rhoTurbFoam version.

I managed to compile the application in 2.2 but I didn't test it, I get also a lot of suspicious warning...

If you are going to test it with OpenFoam 2.2 please keep me posted

Daniele
panara is offline   Reply With Quote

Old   February 16, 2006, 16:22
Default Hi, Daniele, I downloaded y
  #64
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Hi, Daniele,

I downloaded your solver and compiled under OpenFOAM 1.2. The followings are the warnings and errors I got (I will try to see if I can adapt the solver to OpenFOAM 1.2, but, if any one is successfully in adapting the solver to 1.2 first, it will be appreciated if you can post the fix):

SOURCE_DIR=.
SOURCE=conjugateFoam7.C ; g++ -m64 -DlinuxAMD64 -Wall -W -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -ffast-math -DNoRepository -ftemplate-depth-30 -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/cfdTools/compressible -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/cfdTools/general/lnInclude -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/specie/lnInclude -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/thermophysicalModels/basic/lnInclude -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/turbulenceModels -I/home/phsieh/OpenFOAM/OpenFOAM-1.2/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -c $SOURCE -o Make/linuxAMD64Gcc4Opt/conjugateFoam7.o
readPISOControls.H: In function 'int main(int, char**)':
readPISOControls.H:53: warning: use of old-style cast
readPISOControls.H:54: warning: use of old-style cast
pEqn.H:12: error: 'ddt0' is not a member of 'Foam::fvc'
pEqn.H:15: error: 'ddt0' is not a member of 'Foam::fvc'
pEqn.H:40: error: 'ddt0' is not a member of 'Foam::fvc'
pEqn.H:42: error: 'ddt0' is not a member of 'Foam::fvc'
make: *** [Make/linuxAMD64Gcc4Opt/conjugateFoam7.o] Error 1

Pei
hsieh is offline   Reply With Quote

Old   February 16, 2006, 22:46
Default Hi, Pei-Ying, 1. modify Mak
  #65
New Member
 
Masato Otsuki
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 26
Rep Power: 8
otsuki is on a distinguished road
Hi, Pei-Ying,

1. modify Make/options:
EXE_INC = \
-I$(LIB_SRC)/cfdTools/compressible \
-I$(LIB_SRC)/cfdTools/general/lnInclude \
...
2. replace pEqn.H by rhoTurbFoam/pEqn.H
and modify mesh. --> mesh1.
Then you can compile conjugateFoam7 with
OpenFoam-1.2.

You must modify ConjugatePipe/system/fvSchemes
to run the case. I can't run the case yet.

Masato
otsuki is offline   Reply With Quote

Old   February 17, 2006, 05:12
Default Hi Daniele I converted your
  #66
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Hi Daniele

I converted your code to OF1.2 (happy to provide it if someone is interested) but ran into problems when trying it on your case. First iteration is fine, obviously, but in the second timestep the temperature gradient gradT1 is 10e+06, have you seen that before? Consequently the thermodynamics goes ballistic and stop with an error.

//Eric
lillberg is offline   Reply With Quote

Old   February 17, 2006, 06:09
Default Works like a charm... awaiting
  #67
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Works like a charm... awaiting the results...

//E
lillberg is offline   Reply With Quote

Old   February 17, 2006, 09:18
Default Daniele, The results looks
  #68
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Daniele,

The results looks fine, a very neat case to show the ability of OF to solve coupled problems. Is there any validation case with analytical/experimental values to compare with?

//Eric
lillberg is offline   Reply With Quote

Old   February 17, 2006, 09:35
Default Hi, Eric, I ran the case.
  #69
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Hi, Eric,

I ran the case. Used foamToVTK to export two regions, then, read both regions using paraview. The liquid phase has temperature gradient, however, the temperature of the pipe region looked strange (grey color). Did you get the same results? Or how did you post process your results?

Thanks!

Pei
hsieh is offline   Reply With Quote

Old   February 17, 2006, 10:26
Default Hi, Eric, Never mind! I go
  #70
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 317
Rep Power: 9
hsieh is on a distinguished road
Hi, Eric,

Never mind! I got it. I am just not use to multi-regions in paraview yet. The results seem reasonable.

Hi, Daniele,

Great job!

Pei
hsieh is offline   Reply With Quote

Old   March 16, 2006, 15:06
Default Dear all, I am trying to va
  #71
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Dear all,

I am trying to validate the solver for unsteady conjugate flows but I get strange results.

The test case is and hydrodynamically fully developed pipe flow with a wall suddenly set at a different temperature Tw at time t=0. The flow and The wall are at same temperature Ti at time t<0.

here you can see what I get, in the picture there are two different time steps.



It seems that at the solid fluid interface something is wrong... I am not sure if I have imposed the right thermal diffusivity for the solid..

The test case is with alpha_fluid = alpha_solid
(alpha = thermal diffusivity)

and k_solid=10 * k_fluid ( k = thermal conductivity)

I imposed the thermal conductivity ratio and I calculated the thermal diffusivity for the solid as:

alpha_solid=alpha_fluid= mu/(Pr * rho )

mu = 1.84e-5
Pr = 0.7
rho = 0.5 (T = 700 K)

I didn't use mu(T) since I am using constant thermal properties.. is it ok?

Anybody has any suggestion?

Daniele
panara is offline   Reply With Quote

Old   June 7, 2006, 18:33
Default Hi Mattijs, I was trying to
  #72
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hi Mattijs,

I was trying to give a parallel run (using LAM-MPI) to the solver "simpleFoam-twoMeshes" posted by you on Friday, July 01, 2005 in this thread. I came across the following error:
----------------------------------------------
n-1<24686> ssi:boot:base:linear: booting n0 (lionxm150)
n-1<24686> ssi:boot:base:linear: booting n1 (lionxm151)
n-1<24686> ssi:boot:base:linear: finished

LAM 7.1.1 - Indiana University

mpirun: cannot start simpleFoam-TwoMeshes on n0: No such file or directory
-------------------------------------------
I would appreciate any comments on the possible reasons behind the above error.

Thanks!
Regards,
Ankur
ankgupta8um is offline   Reply With Quote

Old   June 8, 2006, 12:36
Default Hi, The problem I had as me
  #73
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hi,

The problem I had as mentioned in the last posting is due to the fact that the executable (simpleFoam-TwoMeshes) was getting placed in $Foam_User_Appbin. Once I changed it to $Foam_Appbin, it was working fine.

-Ankur
ankgupta8um is offline   Reply With Quote

Old   June 8, 2006, 19:02
Default I forgot to mention just for r
  #74
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
I forgot to mention just for records that the code has been validated. There was just a wrong sign of the heat flux at the interface. It is important to pay attention at the wall normals...!! =)

Daniele
panara is offline   Reply With Quote

Old   August 18, 2006, 08:08
Default Hi Daniele, Is the latest cod
  #75
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hi Daniele,
Is the latest code running with OpenFOAM 1.3?
I have troubles to compile conjugateFoam7 with this version. For instance there is no "findRefCell" defined anywere, or at least I coud not find it in the documentation (only findRefCell.H exists as a source file).
It would be very nice if you could post again the solver and the case files on the forum.

Dragos
dmoroian is offline   Reply With Quote

Old   August 18, 2006, 10:41
Default Sorry Dragos but I am using Op
  #76
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Sorry Dragos but I am using OpenFOAM 1.2 and with it I do not have any troubles...

what kind of error message do you get?

Daniele
panara is offline   Reply With Quote

Old   August 18, 2006, 13:07
Default Hi, I'm trying to solve flo
  #77
New Member
 
Helmut Roth
Join Date: Mar 2009
Posts: 23
Rep Power: 8
helmut is on a distinguished road
Hi,

I'm trying to solve flow and temperature on a three region domain consisting of two fluid ducts with square cross section separated by a solid slab of the same size. I'd like to do this by solving fluid flow in the fluid regions, and temperature on the entire domain, but I'm getting some nonphysical values.

I have a mesh of the entire domain and submeshes of the two fluid domains. The latter were generated by the submesh utility using cellSets of the fluid regions. For simplicity, the fluid flow and the material properties are independent of temperature. The velocity fields computed on the fluid region submeshes are transferred to their respective regions of the velocity field U_ALL on the full mesh prior to the temperature calculation, which is coded as

RhoUCp = ( fvc::interpolate(rho_All*U_All*Cp_All) & meshAll.Sf() );
solve ( fvm::div(RhoUCp, T_All) - fvm::laplacian(DT_All, T_All) );

U_All is zero within the slab. The fields rho_ALL, Cp_All, and DT_All are region-wise constant with, respectively, the densities, heat capacities, and thermal conductivities of the three materials/regions. The fluid inlet temperatures are set at 300K, the exterior fluid duct walls are set at 300K, the initial interior fluid duct temperatures are 300K, and the fluid outlet conditions are zero-gradient. The slab exterior boundaries are set at 400K and the slab interior is initialised to 400K. The velocity solutions in the ducts are identical to solutions obtained from simpleFoam, and I've checked the transfer of the velocity fields. Nonphysical temperature values are occurring at the inlets and outlets. Temperatures at the inlets drop below 300K to 291K, while at the outlets there are temperatures in excess of 44500K. (See the attached figures).



Thanks for any ideas,
Helmut
helmut is offline   Reply With Quote

Old   August 21, 2006, 14:39
Default Well that is bad news for me.
  #78
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Well that is bad news for me. I have to check the changes in 1.3 release. Anyway, the error is the following:

dragosm@tirian01:~/OpenFOAM/dragosm-1.3/run/conjugateHeat/conjugateFoam7> wmake
make: Inget behöver göras för "allFiles".
make: "Make/linuxAMD64Gcc4DPOpt/dependencies" är färsk.

SOURCE_DIR=.
SOURCE=conjugateFoam7.C ; g++ -m64 -DlinuxAMD64 -DDP -Wall -W -Wno-unused-parameter -Wold-style-cast -march=opteron -O3 -DNoRepository -ftemplate-depth-30 -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/cfdTools/compressible -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/cfdTools/lnInclude -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/cfdTools/general/lnInclude -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/thermophysicalModels/specie/lnIncl ude -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/thermophysicalModels/basic/lnInclu de -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/turbulenceModels -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude -I/fsd/home/dragosm/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -c $SOURCE -o Make/linuxAMD64Gcc4DPOpt/conjugateFoam7.o
readPISOControls.H:
readPISOControls.H:47: error: findRefCell was not declared in this scope
readPISOControls.H:53: warning: use of old-style cast
readPISOControls.H:54: warning: use of old-style cast
make: *** [Make/linuxAMD64Gcc4DPOpt/conjugateFoam7.o] Fel 1

Thank you for considering my question.
Dragos
dmoroian is offline   Reply With Quote

Old   August 22, 2006, 01:22
Default Something seems to be wrong in
  #79
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Something seems to be wrong in the file readPISOControls.H

Try to start from scratch, you have to copy together rhoTurbFoam and LaplacianFoam the ones that work with OF1.3 (that means also the readPISOControls.H version 1.3).
Then add the additional command like in conjugateFoam7.C and the file createFields.H.
Then you change mesh in mesh1 or mesh2 wherever is needed.
Control also the path in Make/options, they should be more or less a combination of the path in rhoTurbFoam and LaplacianFoam 1.3.
when you compile you can get some error from files that are not in your compiling directory and that use mesh insted of mesh1 or mesh2.
Find them e copy them in your compiling directory
changing mesh in mesh1 or mesh2 and recompile..

Good Luck,

Daniele
panara is offline   Reply With Quote

Old   August 22, 2006, 05:29
Default Here's a fixed version of cunj
  #80
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Here's a fixed version of cunjugateFoam7 compiling under OF 1.3.

conjugateFoam7_of13.tgz

findRefCell is not used anymore, so setRefCell will use the cellnumber given in the PISO dict.

Regards

//Eric
lillberg 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
heat conduction in solid - mismatch to exp. res. Ralf Schmidt FLUENT 1 December 9, 2008 09:34
Solid mesh for heat conduction Munni FLUENT 1 December 12, 2006 13:24
heat conduction in a solid francesco FLUENT 0 May 27, 2004 18:00
Heat conduction in a solid domain Rene CFX 0 October 20, 2003 03:33
Heat conduction in a solid domain S. Balasubramanyam CFX 10 October 14, 2003 08:57


All times are GMT -4. The time now is 06:29.