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   September 7, 2007, 07:00
Default Hello Oscar, I looked at yo
  #101
Member
 
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8
ariorus is on a distinguished road
Hello Oscar,

I looked at your code and I have a question about it.


Since the two equations are solved one after the other and not at the same time it is necessary to solve them many times such that the proper boundary conditions at the interface be satisfied, and you do this.
So you first solve the two solid equations and then reset the bc values of the coupled patches according to what is specified in the 0/T files.
But as far as I understood you reset the gradient value in solid2, if fixedGradient is specified in solid2 0/T file, and the temperature value in solid1 if fixedValue is specified in solid1 0/T file. What happens if you put for instance fixedGradient in both solid1 and solid2 coupled patch? Do you reset only the gradient value and not the temperature?

I may be wrong (if so please correct me) but I think that at every time>0 at the interface between cells of the 2 solids you should have always that the temperature and the heat flux be the same. Did you check this?

You could also try to see what happens playing with conductivity (if a conductivity for a solid is equal to zero you should recover a fixed temperature bc for the other).

I think that an analytical solution should be not too difficult to be found, for instance you could set up a 1D problem.

Ciao.

Rosario
ariorus is offline   Reply With Quote

Old   September 8, 2007, 19:46
Default Hi Rosario, thanks for your c
  #102
New Member
 
Oscar G
Join Date: Mar 2009
Location: Bogotá, Bogotá, Colombia
Posts: 27
Rep Power: 8
oscar_j is on a distinguished road
Hi Rosario,
thanks for your comments.

My first idea in order to couple the two solids is to suposse no heat generation in the interface, so I want to couple the solids like Daniele propose:

T1=T2, at interface
dT2/dn=-k1/k2*dT1/dn, at interface

I think if you put fixedGradient in the two solids it could happen an error when the code reads a patch defined like fixedGradient initially and then it try to set fixedValue.

The solver hasnt been tested yet.
Any help and comment I appreciate so much.

Thanks a lot!
Oscar
oscar_j is offline   Reply With Quote

Old   September 9, 2007, 15:44
Default Hi Rosario, I post the fir
  #103
New Member
 
Oscar G
Join Date: Mar 2009
Location: Bogotá, Bogotá, Colombia
Posts: 27
Rep Power: 8
oscar_j is on a distinguished road
Hi Rosario,

I post the first results I have obtained with twomeshes Solver. The case consists in two coupled cubes with 1 meter of side length and same material. The initial temperatures are T1=285K and T2=293K. With these considerations, the temperature of thermal balance would be T=289K. The image is a cross-sectional of the cubes.



Although the thermal balance is obtained, in the interface the temperature distribution has a rare variation around the thermal balance temperature, Any idea how could I make better the code?

Regards
Oscar
oscar_j is offline   Reply With Quote

Old   September 9, 2007, 15:48
Default Sorry http://www.cfd-online.co
  #104
New Member
 
Oscar G
Join Date: Mar 2009
Location: Bogotá, Bogotá, Colombia
Posts: 27
Rep Power: 8
oscar_j is on a distinguished road
Sorry
This is the image:

oscar_j is offline   Reply With Quote

Old   September 21, 2007, 12:21
Default I'm trying to use openFoam to
  #105
connclark
Guest
 
Posts: n/a
I'm trying to use openFoam to simulate cooling of electronics by convection currents in a case as well as the heat dissipated by the case by convection as well.

Unfortunately, I can't seem to get any of these solvers posted to this thread to work with OpenFOAM 1.4.1 :-(

Also I was wondering about how one could do a continuous power input to a solid instead of specifying a temperature.

Forgive me I'm new to openfoam.
  Reply With Quote

Old   September 22, 2007, 04:41
Default Dear Clark, search the open
  #106
Member
 
sradl's Avatar
 
Stefan Radl
Join Date: Mar 2009
Location: Graz, Austria
Posts: 82
Rep Power: 9
sradl is on a distinguished road
Dear Clark,

search the openfoamwiki for conjugate heat transfer - the solvers posted there should also work with OF 1.4.1 (not tested by myself).

Specifying a continous power input (e.g. W/m2) means that you will have a constant temperature gradient in the solid at the interface. Thus, dT/dx = q/lambda, where lambda is the heat conductivity of the solid. Specifying a constant gradient at the interface is a standard OF boundary condition :-)

br
Stefan
sradl is offline   Reply With Quote

Old   September 22, 2007, 04:42
Default sorry, of course heat flows ac
  #107
Member
 
sradl's Avatar
 
Stefan Radl
Join Date: Mar 2009
Location: Graz, Austria
Posts: 82
Rep Power: 9
sradl is on a distinguished road
sorry, of course heat flows across the negative temperature gradient:

q=-dT/dx.lambda

cheers
stefan
sradl is offline   Reply With Quote

Old   September 24, 2007, 12:52
Default Stefan, I have tried to get
  #108
connclark
Guest
 
Posts: n/a
Stefan,

I have tried to get the example of the conjugate heat transfer found here http://openfoamwiki.net/index.php/HeatTransfer
to work. I was able to hack the code so it compiled, however there are differences in the case file directory structure that I can't figure out how to solve. The main issue being how to combine the fluid region and the solid region in the constant directory so that the 1.4.1 based solver can read it.

Also note that the src tar ball for the pseudo heat solver doesn't contain the code for it.
  Reply With Quote

Old   September 26, 2007, 01:15
Default Dear All I am a new user of
  #109
New Member
 
Armin Hosseinian
Join Date: Mar 2009
Location: Perth, Western Australia, Australia
Posts: 17
Rep Power: 8
armin_h is on a distinguished road
Dear All

I am a new user of OpenFoam as phd petroleum candidate, and i need to simulate fluid flow through the pipe , which should be cilynder.

I will be appreciate if someone let me know how can i create pipe shape in OpenFoam, and which part of OpenFoam Will help me to do so.

Many Thx in advance
armin_h is offline   Reply With Quote

Old   September 29, 2007, 14:44
Default Dear Clark, it should be ea
  #110
Member
 
sradl's Avatar
 
Stefan Radl
Join Date: Mar 2009
Location: Graz, Austria
Posts: 82
Rep Power: 9
sradl is on a distinguished road
Dear Clark,

it should be easy to find the code section in 1.4.1 where the source directory is defined for reading the mesh info. Just study the code - you should have a "solidRegion" and a "fluidRegion" directory under your case/constant directory; both solidRegion and fluidRegion should have a "polyMesh" dir.

In your case you possibly will need two liquid regions (the air inside and outside the case) as well as the metal. So I guess you need a major review of the solver.

br
Stefan Radl
sradl is offline   Reply With Quote

Old   October 10, 2007, 11:27
Default Dear Forum, My question is
  #111
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
Dear Forum,

My question is not a convection one but a coupling one and this thread is the more interresting one about coupling.
I'm doing a solver for coupling 2 fluids regions. In my case, I want to couple a channelOodles region and a Oodles one. It's usefull is you want to get turbulent flow without adding white noise.
I used a lot your upper convection solver to do that.

but, I still have one problem in the createFields.H files:

createFields.H:65: error: no matching function for call to 'Foam::dictionary::New(Foam::volVectorField&, Foam::surfaceScalarField&)'
/craya/big/duprat/OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/lnInclude/dictionary.H:10 5: note: candidates are: static Foam::autoPtr<foam::dictionary> Foam::dictionary::New(Foam::Istream&)


it correspond to the following source:

autoPtr<transportmodel> laminarTransport1
(
transportModel::New
(
U1,
phi1
)
);

autoPtr<lesmodel> sgsModel1
(
LESmodel::New
(
U1,
phi1,
laminarTransport1()
)
);

in the Mattijs Janssens upper code, there is still line like that.
So my question is, Is there any constructor to create in the dictionnary files (.C and .H) or I made a mistake ther ?

Thank you for helping,
Regards,

Cedric
cedric_duprat is offline   Reply With Quote

Old   October 11, 2007, 06:11
Default If you want fully developed in
  #112
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
If you want fully developed inlet, it is much easier to use the directMappedFixedValue boundary to map internal fields to the boundary than to use a 2 mesh solution.
eugene is offline   Reply With Quote

Old   October 11, 2007, 08:22
Default Hi Eugene, that is interestin
  #113
Senior Member
 
Daniele Panara
Join Date: Mar 2009
Posts: 101
Rep Power: 8
panara is on a distinguished road
Hi Eugene,
that is interesting, can you post an example of the blockmesh file with the internal field and ,for example, of the U file with the directMappedFixedValue BC?

I would like to simulate a long pipe with an oscillating flow and a section with heat transfer..

So my idea would be to have a first part of the channel with 'internal periodic BC' which will feed the second part with the heat transfer..

I oscillate the flow with a source term in the momentum equation.

I guess I am going to have problems when the flow reverse.. but I will think about that later on.. =)

For now, it is interesting for me just to try a pulsating channel (no reverse flow) and in this case it should work fine..

Daniele
panara is offline   Reply With Quote

Old   October 11, 2007, 09:40
Default Sure. In this example "inlet"
  #114
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Sure. In this example "inlet" refers to the patch that uses internal mapping:

1. In constant/polyMesh/boundary

inlet
{
type directMappedPatch;
nFaces #;
startFace #;
offset (<offset> 0 0 1)
}

2. Normally you need to map velocity and turbulent properties. Thus in U file boundary section:

inlet
{
type directMappedFixedValue;
value (<placeholder> 0 0 0);
average (<target> 0 0 2);
}

The "average" entry is not compulsory. For example a hypothetical k field inlet would look like this:

inlet
{
type directMappedFixedValue;
value (<placeholder> 1e-10);
}

Unfortunately, the "directMappedPatch" boundary mesh type is not yet supported by decomposePar and other mesh manipulation utilities. So if you want to run in parallel, you will have to manually edit the processor boundary files to add the directMappedPatch entries.
eugene is offline   Reply With Quote

Old   October 11, 2007, 09:41
Default Hi Eugene and Daniele, well
  #115
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
Hi Eugene and Daniele,

well, maybe you're write, I will try to use the directMappedFixedValue BC but, before trying, could you explain us what is it please. Because, I the forum, the "directMappedFixedValue" was cited only 3 times now : Eugene 1 today, Daniele 1 few minutes ago and me .... now :o)

more generaly, I think a coupling solver for two fluid will be also the first step for a RANS / LES coupling.

Cedric
cedric_duprat is offline   Reply With Quote

Old   October 11, 2007, 09:43
Default oups ... I'm a little bit lat
  #116
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
oups ...
I'm a little bit late... :o)
Thank you Eugene
cedric_duprat is offline   Reply With Quote

Old   November 7, 2007, 22:15
Default Hi everybody, I would want
  #117
New Member
 
Oscar G
Join Date: Mar 2009
Location: Bogotá, Bogotá, Colombia
Posts: 27
Rep Power: 8
oscar_j is on a distinguished road
Hi everybody,

I would want to calculate the mean temperature in a fluid and solid, is there any function or way in order to do that?, I have worked on buoyantfoam for the fluid and laplacianfoam for the solid.

Thanks!
Oscar
oscar_j is offline   Reply With Quote

Old   November 8, 2007, 05:08
Default Hi Oscar, There is e.g.
  #118
Senior Member
 
Thomas Jung
Join Date: Mar 2009
Posts: 100
Rep Power: 8
tehache is on a distinguished road
Hi Oscar,

There is e.g.

fvc::domainIntegrate(T))

to integrate field T
tehache is offline   Reply With Quote

Old   April 7, 2008, 05:05
Default hi, i have a case with 2 inle
  #119
Member
 
davey david
Join Date: Mar 2009
Posts: 54
Rep Power: 8
suredross is on a distinguished road
hi,
i have a case with 2 inlets and an outlet,with 2 different liquids at the inlets.which equation and how do i couple it to work in openfoam?i tried the icoFoam solver but something seems wrong?
i am new to OF and need help,desperately!
thanks
david
suredross is offline   Reply With Quote

Old   April 7, 2008, 05:58
Default Hi Davey Have a look at the
  #120
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Davey

Have a look at the damBreak case in the User Guide. It is using the interFoam solver, which solves for a two-phase flow.

You say you are having two inlets, is it one inlet per fluid, or is there a mixture of the fluids in either inlet?
If the first is the case, you simply specify in the gamma file in /0/gamma that inlet1 has the value 1 and that inlet2 has the value 0. If you have a mixture, it might become somewhat more difficult - I don't know if there are any tools which you could use directly or if you need to program something yourself.

Best regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj 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 18:19.