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

chtMultiRegionSimpleFoam with heat source not at boundary

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2013, 06:07
Default chtMultiRegionSimpleFoam with heat source not at boundary
  #1
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi Foamers,

Just a quick question - I have noticed that the heat sources for the chtMultiRegionSimpleFoam tutorials are applied at the patches.

I followed the tutorial and tried a case where an object (a cube for example) is suspended in a fluid domain. When I tried to make the cube a heat source, I have not been able to (rather the solver does not seem to take it into account at all).

I have been looking through the threads in this forum but have not found anything that addresses this question. Anyone knows how to overcome this issue? Is this a limitation of the solver or am I missing something?

Any advise would be much appreciated.

Thanks very much!

Regards,

Antimony
Antimony is offline   Reply With Quote

Old   November 28, 2013, 03:21
Default heat source with compressible::turbulentTemperatureCoupledBaffleMix ed possible?
  #2
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi All,

I do not know if my question was clear or not and so I thought I would rephrase and ask the question:

My problem is basically this: I have a solid box (called box) in a fluid domain (called domain0). How do I assign a heat flux any heat source on the surface separating the solid and the fluid regions? I need to understand the temperature distribution in both regions.

How do I assign a heat flux or a heat source to the baffle, especially to the compressible::turbulentTemperatureCoupledBaffleMix ed type?

Or can I use something like compressible::turbulentHeatFluxTemperature and specify a heat source?

Any ideas on this are much appreciated.

Thanks for your time!

Regards,

Antimony

Last edited by Antimony; November 28, 2013 at 03:22. Reason: typo in the title
Antimony is offline   Reply With Quote

Old   November 29, 2013, 06:49
Default
  #3
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 311
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi Antimony,

I would not be sure about changing the boundary, it does not look like it is straightforward to do so. I think you could use the fvOptions framework to specify a heat source for the entire solid region (or part of it). The heattransfer from/to the fluid would than be done with the turbulentTemperatureCoupledBaffleMixed on the boundary.

Good luck,
Tom
tomf is offline   Reply With Quote

Old   November 29, 2013, 07:42
Default
  #4
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi Tom,

Thanks very much for your reply! At least now I have some idea on how I should go about thinking this problem.

I had tried the turbulentHeatFluxTemperature method and specified the same flux on both sides. The results however were incorrect at the interface. Unfortunately at the interface, depending on whether you are at the solid side or the fluid side, the temperatures are different and the difference is substantial (>30K) for a heat source of say 500 W/m2 (just a test value). Whichever way you look at it, the temperature at the interface has to be one value right?

Couple of added questions though:
1. Based on what you have suggested, it would seem that even if I wanted to apply a heat flux I would probably have to convert it and put it in as a volume source right?

2. I am currently on OF 2.1.x. Unfortunately, at this moment, I cannot upgrade to release 2.2.x and consequently fvOptions isn't a choice for me, at least for now. Any suggestions how to apply constant volume source without using the fvOptions? I am guessing something like what is done in the damBreak example for interFoam, but I am not sure how to put in the volume source. Unless of course I have to tinker with the solver itself?

3. I was reading through some of the older posts as well, especially the ones from OF v 1.6. There they had something called solidWallHeatFluxTemperature and it seems like they were able to specify fluxes. From all the posts on that, it seems to be a very handy tool, which unfortunately they removed/replaced with the temperatureCoupledBaffle from OF v 2.0. Given that it was a very useful thing, I would think that they would have incorporated it somewhere in the new BC, no?

4. Finally, do you have any idea about what the refValue, refGradient and valueFraction actually do and how they should be input for turbulentTemperatureCoupledBaffleMixed? I tried looking into the source but I really cannot understand it. And if I specify only one of the parameters, the solver won't work because it needs all three as inputs. I thought of specifying temperature on one side and heat flux on the other just to see what happens, but because of the error, that could not be done.

Apologies for the long post.

Once again, thanks for your views. Really appreciate them.

Regards,

Antimony
Antimony is offline   Reply With Quote

Old   November 29, 2013, 11:43
Default
  #5
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Delft, Netherlands
Posts: 311
Rep Power: 12
tomf is on a distinguished road
Send a message via MSN to tomf Send a message via Skype™ to tomf
Hi,

I don't think I can help you on everything, but can at least try to answer your questions out of the top of my head:

1. Yes

2. Do not know this by heart, except for indeed modifying the solver

3. I do not know that particular boundary condition, so can not help you here.

4. From the tutorial (of22x) I see something like this for the boundary condition:

Code:
    heater_to_bottomAir
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        neighbourFieldName T;
        kappa           solidThermo;
        kappaName       none;
    }
For of21x I see something similar, so I do not know why you would need any of "refValue, refGradient, valueFraction"? They are determined by the solver based on the input you give in the boundary condition. I think they refer to some code behind the mixed type boundary condition. So I do not think you should need to set any of these values.

Hope this helps,
regards,
Tom
tomf is offline   Reply With Quote

Old   December 1, 2013, 23:58
Default
  #6
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi Tom,

Thanks very much once again for your replies! It will be very useful and once again gives me a direction to go in.

I will look into this based on what you have said.

Just to let you know: for the turbulentTemperatureCoupledBaffleMixed boundary condition, there seems to be the refValue, refGradient etc. I agree with you that they might be calculated by the solver itself, but was just curious if you or anyone else had any idea about those parameters.

Once again thanks very much and if I do manage to get something for this, will post back here.

Regards,

Antimony
Antimony is offline   Reply With Quote

Old   January 1, 2014, 22:27
Default
  #7
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi,

Happy New Year to you guys!

Just a quick question (and this refers back to an older post of mine on a similar topic: chtMultiRegionSimpleFoam with heat source not at boundary) - Have either of you tried to prescribe a heat flux at the boundary?

I hope I am not spamming. I would just like to know if either of you have looked into this before and/or have any suggestions for the same.

Thanks very much!

Regards,

Antimony

[Moderator note: This post and the following 2 posts have been moved from this thread: http://www.cfd-online.com/Forums/ope...penfoam-2.html - Reason: to avoid getting an overlap of different conversations.]

Last edited by wyldckat; January 5, 2014 at 09:51. Reason: see "Moderator note:"
Antimony is offline   Reply With Quote

Old   January 2, 2014, 14:19
Default
  #8
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 4
skuznet is on a distinguished road
Hi Antimony!

I'm prescribing fixed temperature now, but will need actually to prescribe a heat flux instead.
I'm not sure if it is possible to prescribe fixed flux directly in OF, but one can prescribe temperature gradient using fixedGradient.

Did you try to prescribe it already?

Sergey
skuznet is offline   Reply With Quote

Old   January 3, 2014, 04:01
Default
  #9
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Hi Sergey,

For some of the other problems that I was working on, I used compressible::turbulentHeatFluxTemperature because it allows you to choose between heat flux (W/m2) and heat source (W).

For the cht problem that I am working, I basically want to prescribe a heat flux on the interface between the solid and the fluid. Unfortunately, when I use the compressible::turbulentHeatFluxTemperature, there is a big discontinuity in the temperature of the interface depending on where it is measured.

One of the suggestions that I had gotten on this forum was that I use a volumetric heat source, but if I do, it would change the way the heat propagates through the solid.

As a result, I am currently stuck.

If you have any ideas, I would be happy to try them out. I am currently working with OF 2.1.x BTW

Regards,

Antimony
Antimony is offline   Reply With Quote

Old   January 5, 2014, 10:07
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Antimony: I've moved the 3 posts above, because it was getting a bit confusing in the other thread - http://www.cfd-online.com/Forums/ope...-openfoam.html - and this seemed a better place to discuss this issue.

A few questions about your problem, very similar to the questions I had asked Sergey on the other thread:
  1. Do you have the turbulence modelling turned on? If so, which one?
  2. What is the mesh profile of your case, between wall and fluid? Is the mesh uniform or thinner closer to the wall?
  3. What is the contact area and the flow speed of the fluid?
  4. Do you have an analytical solution of this case, to base your conclusions on?
  5. Have you tried reproducing this issue with this example case: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D - it's a good simpler case to manipulate/change and to try additional solutions and can more easily be shared. And best of all, there are analytical solutions for the "plane wall" scenario
Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   January 5, 2014, 23:50
Default
  #11
Senior Member
 
Join Date: Aug 2013
Posts: 180
Rep Power: 4
Antimony is on a distinguished road
Dear Bruno,

Thank you for your reply and for moving the posts to a better location!

Maybe I reply to your last question first? Think it will be better to start from there.

Yes, I have downloaded and tried the planeWall2D problem. In fact I used that as the case to understand how the chtMultiRegionSimpleFoam solver works, especially the regions part. Thank you very much for that! Has been very helpful.

Unfortunately though, the boundary conditions for that project are different from what I would want.

I have attached a snapshot of the type of geometry that I am using where there is a solid immersed in a fluid. As you can see the type of BC that I want on the interface is not the same as the planeWall2D tutorial. In fact, in the default tutorials in OF for chtMultiRegionSimpleFoam also, there isn't any example that uses heat flux, especially not on the interface and that is what I am chasing after.

I would be grateful for any pointers that you might have. Some of the earlier suggestions are to use a volumetric heat source. As far as possible, I do not want to do that because I am interested in knowing how the heat transfer through the solid happens.

To answer your other questions:
1. Yes I have included turbulence and have used the k-w SST model.
2. I created refinement regions around the solid and made the mesh there finer than the others.
3. The fluid is stationary. I understand that I cannot set the speed to zero, especially when using the ideal gas model for air and so I had set the internalField value to (0.01 0 0).
4. I haven't worked out an analytical solution for this.

Once again thanks very much for your advise and help!

Best Regards,

Antimony
Attached Images
File Type: jpg HeatFluxGeometry.jpg (22.7 KB, 71 views)

Last edited by Antimony; January 5, 2014 at 23:52. Reason: Incorrect way of uploading image
Antimony is offline   Reply With Quote

Old   January 24, 2014, 14:01
Default
  #12
Member
 
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 9
micpage18 is on a distinguished road
Hi Antimony,

I have a case similar at yours. Do you succeed to set a volumetric heat source?

Thank you,
__________________
Michael Page
michael.page@simu-k.com
Simu-K inc.
www.simu-k.com
micpage18 is offline   Reply With Quote

Old   January 26, 2014, 16:48
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Antimony: Sorry, I've been busy these past few weeks and had a long list of threads here on the forum that I wanted to answer to...

OK, I only managed to give a quick very read to your posts and I think that the boundary condition "externalWallHeatFluxTemperature" might be what you're looking for. Instructions on how to use it are in the comment part in the file revealed by this command:
Code:
echo $FOAM_SRC/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/externalWallHeatFluxTemperature/externalWallHeatFluxTemperatureFvPatchScalarField.H
When in doubt, have a look at the boundary conditions in display here: http://foam.sourceforge.net/docs/cpp/modules.html

The problem is that with this boundary condition, you cannot use a meshed region for the solid itself.

The other possibility is to rely on "fvOptions" for creating special cell-zone manipulations, such as those exemplified in the tutorial "heatTransfer/chtMultiRegionSimpleFoam/heatExchanger". You can find several examples by running:
Code:
find $FOAM_TUTORIALS -name "fvOptions"
Also browse through the "fvOptions" types available, listed at the folders indicated by the following commands:
Code:
echo $FOAM_SRC/fvOptions/constraints/
echo $FOAM_SRC/fvOptions/sources/
Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   January 27, 2014, 13:18
Default
  #14
New Member
 
Christian Renaux
Join Date: Dec 2012
Posts: 1
Rep Power: 0
kortak is on a distinguished road
Hi,

I'am having the same kind of problem to solve, where I would like to simulate the solar energy heat flux on one wall surface. I am a novice on openfoam and will try very soon this kind of simulation...so I will get back on this thread if I have some good or bad results.

Cheers.
kortak is offline   Reply With Quote

Reply

Tags
chtmultiregionsimplefoam, heat source

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
swak4foam building problem GGerber OpenFOAM Installation 54 April 24, 2015 16:02
Radiation interface hinca CFX 15 January 26, 2014 18:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
friction forces icoFoam ofslcm OpenFOAM 3 April 7, 2012 10:57
wall heat flux or boundary source of energy??? Albi CFX 1 May 4, 2007 11:25


All times are GMT -4. The time now is 20:43.