|
[Sponsors] |
August 3, 2010, 10:07 |
|
#21 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
This "WE" implies that there is someone else loosing sleeping hours for this as me???
Do you also need the solver? I will email them as soon as possible. thanks mad Last edited by maddalena; August 3, 2010 at 10:21. Reason: adding files |
|
August 4, 2010, 06:51 |
|
#22 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Hi mad,
I've looked at it. The problem maybe the symmetry/zeroGradient condition on the left side of cube1, that makes T unbounded, while a fixedValue works. My advise will be to try a cube2-cube1-cube 2 configuration. I opened this case and the tutorial, the cube case looks 10 times greater than it should be, but maybe is a paraview ocus-pocus. let me know Andrea |
|
August 4, 2010, 07:11 |
|
#23 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello Andrea,
Quote:
And this is the logical conclusion... Ok, I will report it as soon as possible. What does it mean? cube1 is a cube of 1 meter long. It seems to me that it is like that, no? Or did you compare it with the size of the tutorial? I have made them independently, so maybe I should scale my case to match the tutorial dimensions... Thanks for your support, at least now I have a possible answer to the problem! ciao mad |
||
August 4, 2010, 07:22 |
|
#24 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Code:
cube1 is a cube of 1 meter long. It seems to me that it is like that, no? Or did you compare it with the size of the tutorial? I have made them independently, so maybe I should scale my case to match the tutorial dimensions... Code:
Thanks for your support, at least now I have a possible answer to the problem! ok |
|
August 4, 2010, 11:12 |
|
#25 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hello,
guess what??? It is not working! I have the same results as the cube1-cube2 + symmetry. but... If I use a condition like the one shown in the attached figure... well, everything works! It seems like the solver needs a fixedValue somewhere in the domain to limit the heat source contribution... Indeed... coming back to the modified tutorial example. If you modify the minY BC from fixedValue 500K (or 300K) to zeroGradient BC, (and set U 0 0 0 in the fluid regions) well... The time vs temperature is ok in the first 100 simulated seconds, but it becomes linear after on! Thus it is not the "symmetry" or the "cyclic" or some special condition that does not work, but it is a "heat source limitation" problems. I am going to think to it. Does it has any physical meaning connected with the BC we are fixing or is it a computational problem? What is your opinion on that? mad Last edited by maddalena; August 4, 2010 at 11:56. |
|
August 4, 2010, 12:35 |
|
#26 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Hi,
I agree, but maybe is more subtle than this. Of course source should be limited, but putting a fixedValue on the left side of cube1 and putting zeroGradient on the right of cube2 just works fine... hence, in my opinion, coupling condition misbehaves... Andrea |
|
August 5, 2010, 06:24 |
|
#27 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hi Andrea,
Quote:
One step more... I created a new case, like the cube2-cube1-cube2 case of yesterday and added a very large solid surrounding domain, where I fixed the temperature. Something similar is shown in the attached figure. In this case, we have NO BC on cube1, and its solution depends only on what is happening there. In addition, there is no involving convection, that may represent an additional problem. Now, we have two hypothesis on why the modified version of chtMultiRegionFoam fails:
After running as usual, I have result as usual: linear time vs temperature, hence 2 is true and, as you suggested yesterday,What I cannot explain is why Robertas has a similar case over here, and she claims to have it running... Unfortunately, the case needs some modifications to run. Therefore, we are at the same point of the 20th of July, when I started this thread. How to improve the coupling condition? Or, is there a way to limit the heat source without fixing the temperature on one side of it? regards, mad Last edited by maddalena; August 5, 2010 at 08:46. |
||
August 26, 2010, 10:57 |
|
#28 |
Member
Join Date: Nov 2009
Location: Germany
Posts: 96
Rep Power: 17 |
Hi mad,
I asked the OF support team about the heat source issue. They told me I should take a look at the porousExplicitSourceReactingParcelFoam solver in OF-1.7.x There is a energy source term in createExplicitSources.H: Code:
Info<< "Creating energy source\n" << endl; scalarTimeActivatedExplicitSourceList energySource ( "energy", mesh, dimEnergy/dimTime/dimVolume, "h" ); Regards, Toni |
|
August 26, 2010, 17:01 |
|
#29 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Ehi!
Quote:
Of course, I will have a look to it during the next week or so. And please report everything. The three of us can do a good job, I hope... mad |
||
September 2, 2010, 09:30 |
|
#30 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Hi Toni,
I looked at the file you pointed out. It seems that the createExplicitSources.H, which recalls timeActivateExplicitSource.H, is used only to define a heat source that can be activated / deactivated whenever you need it. In my case, the heat source is on and does not change for all the time, so this approach seems useless. Indeed the explicit source can be defined as I posted above. In any case, Andrea and I found out that is the coupling condition that does not work properly when defining a heat source and not fix at least one of the boundary values. If the temperature is fixed in one of the boundaries, the heat source defined as above gives reasonable results. The problem sounds deeper than it looks like. Hope I can still get some sort of support from the community, but at the moment none has suggested improvement for the coupling yet. Regards, mad |
|
September 10, 2010, 11:38 |
|
#31 |
Member
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 16 |
Hi,
I will take a look at this also, can you send me the solver you have for now ??? You can send it to: fc [at] canesin [dot] com My problem is a little like yours, I have to add an heat source term that reads a variable cp and a variable value that both depends on another equation I solve in the domain.. (it is a triple coupled problem, magnetic+heat+fluid). I will be back in here for the next developments of my solver... hope to work together. |
|
September 10, 2010, 11:48 |
|
#32 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
||
September 16, 2010, 03:37 |
|
#33 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
||
September 16, 2010, 23:06 |
|
#34 |
Member
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 16 |
I have run a preprocessor in it and at the moment I'm trying to understand better the solver.
I agree it seams to do the interface like Patankar book. |
|
September 26, 2010, 03:27 |
|
#35 |
Member
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 16 |
I have added the source term explicit to the solid equation.. I will reproduce from memory the steps here, so I maybe type wrong some code.. I have changed little the solid, but a lot the fluid.. I'm trying to setup some validation cases now.. as soon as I do that will be back here.
tmp<fvScalarMatrix> TEqn ( fvm::ddt(rho*cp, T) - fvm::laplacian(K, T) - S ); Then added a field to it: PrtList<volScalarField> Ss(solidRegions.size()); Ss.set ( i, new volScalarField, IOobject ... ) ... In fact have copied temperature T field and just changed to "S". Then I have changed the flow solver to a incompressible one and removed the PIMPLE loop to a PISO one... now I'm trying to validate with Blasius and planewall.. but I'm having some problems with mesh =/ ... |
|
September 26, 2010, 08:12 |
|
#36 | |
Senior Member
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 334
Rep Power: 18 |
Hi, Canesin,
I am interested in using incompressible solver for fluid in stead of the compressible solver in the current chtMultiRegionFoam solver. I am wondering if you can send me your solver so that I can learn from you? What is your reason for using PISO instead of PIMPLE? Pei phsieh2005@yahoo.com Quote:
|
||
September 26, 2010, 15:22 |
|
#37 | |
Member
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 16 |
Quote:
I`m really sorry for not being able to send my solver.. I have an confidentiality agreement with the sponsor of my project .. But as soon as I have submited an paper to some journal I can publish some code here.. I have used an PISO loop because my problem is not steady-state, it has no steady-state configuration, it can be only determined an periodic developed region... In that case I use an PISO loop since PIMPLE is only to permit the use of large time-step, with don't make sence for me.. removing the PIMPLE to a PISO loop I can remove the outer loop (the "nOuterCorr" for loop) and improve the speedy of the solver. |
||
September 26, 2010, 17:53 |
|
#38 |
Senior Member
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 334
Rep Power: 18 |
Thanks Canesin!
Pei |
|
October 26, 2010, 21:30 |
|
#39 |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Hi Maddalena and Andrea,
Could you please show me how to compute the wall heat flux at every iteration when using the chtMultiRegionSimpleFoam (OF 1.7.0)? I am a complete beginner with OpenFoam, and absolutely weak with C++. Thank you very much. Best Regards, Stefano
__________________
Stefano Wahono Defence Science and Technology Organisation Propulsion Systems |
|
October 27, 2010, 03:39 |
|
#40 | |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 |
Quote:
I commented the if selection while leaving uncommented the inner test in solidWallHeatFluxTemperature. Something like: Code:
// if (debug) // { ... ... // } mad |
||
Tags |
chtmultiregionfoam, coupling, heat source, interface |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Moving heat Source | AB | FLUENT | 2 | January 30, 2012 08:06 |
Version 15 on Mac OS X | gschaider | OpenFOAM Installation | 113 | December 2, 2009 11:23 |
moving heat source | Mehdi | FLUENT | 0 | March 24, 2008 18:32 |
how to define volme heat source in udf ? | wanghong | FLUENT | 0 | February 24, 2006 04:53 |
heat source in a domain | aydin | FLUENT | 0 | January 3, 2003 08:01 |