|
[Sponsors] |
Question about temperature boundary condition |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 12, 2014, 05:25 |
Question about temperature boundary condition
|
#1 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
I am simulating a simple case of fluid heated by a hot pipe with chtmultiregionFoam. I do not want to impose any temperature boundary condition at the outlet and observe rise in the temperature of the fluid as it moves from inlet to outlet.
What condition I must use?? Here are contents of my T file. Code:
boundaryField { inlet { type fixedValue; value uniform 278;//300;// } outlet { type inletOutlet; value uniform 278;//300;// inletValue uniform 278;//300;// } innerfluid2pipe { type compressible::turbulentTemperatureCoupledBaffleMixed; value uniform 278;//300;// neighbourFieldName T; kappa fluidThermo; kappaName none; } } |
|
March 12, 2014, 10:38 |
|
#2 |
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
I assume this is your T file for the fluid region. Therefore the T file of the solid regions is missing.
Can you specify how you process the multiple regions? Usually the splitMeshRegions utility creates patches named <solidRegion_i>_to_<*> and <fluidRegion_j>_to_<*>. This has obviously not happend in your case, but might be OK, if you use third party software for mesh generation, e.g. enGrid does split the regions with its export function. The next step would be to clarify where your heat source and heat sink is. Otherwise you end up with an isothermal domain. |
|
March 13, 2014, 08:29 |
|
#3 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
Thanks for the reply.
My other T file looks this Code:
boundaryField { outerwalls { type fixedValue; value uniform 300;// } pipe2 innerfluid { type compressible::turbulentTemperatureCoupledBaffleMixed; value uniform 278;//300;// neighbourFieldName T; kappa fluidThermo; kappaName none; } } But what it has to do will the other T files?? Am just curious. About the mesh creation: I create my mesh in Ansys meshing, import it in fluent, delete interface, convert the interface to interior, save case, convert case file to foam, and use splitmeshregion. This gives me three regions. |
|
March 13, 2014, 08:55 |
|
#4 |
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
I'm not familiar with your mesh generation process, but it seems to work fine.
How do you get 3 regions? You have got the fluid inside the pipe and the pipe itself. Where is the third one? A surrounding fluid? With respect to your fluid T file: inlet: fixedValue -> 278K set outlet: inletOutlet -> zeroGradient, if the flux vector is pointing outwards your boundary patch face and fixedValue (in your case 278K) in case of backflow, i.e. the flux is pointing inwards. innerfluid2pipe: thermally coupled This looks so far reasonable. Looking at the T file for your solid, I recognize, that you specify at pipe2innerfluid, that the solid kappa is the same as the fluid kappa, i.e. I would expect: kappa -> solidThermo. By applying fixedValue 300K to the outerwalls patch you create a heat source. The heat is then transported by conduction (depending on the thermal conductivity of your solid) to the pipe2innerfluid patch, which is thermally coupled with your fluid, making the fluid the heat sink. Given that the fluid is kept at 278K at the inlet, only a small increase in temperature will be observed at the outlet. So can you explain in detail, what exactly your problem is? |
|
March 14, 2014, 02:39 |
|
#5 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
Thank you for your comments.
Sorry i described mesh generation for some other case. I have 2 regions one fluid and one is pipe. The pipe is hot (relative to fluid) and the hot pipe heats up the cold fluid. I ran some test cases and they seem to be going fine. No other errors and the temperature of the fluid coming out at the outlet also seems reasonable. My concern was that since I am putting a temperature value for the outlet (value uniform 278 the temperature would remain 278 and not increase. Next I am planning to extend it to three and more regions for heat exchange. Right now I am just ensuring that everything works with this basic case. |
|
March 14, 2014, 02:52 |
|
#6 |
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
You are welcome
|
|
March 14, 2014, 02:53 |
|
#7 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
I copied that condition from tutorial 'multiRegionHeater' and 'multiRegionLiquidHeater'. Could you please elaborate on the reason for using ' kappa -> solidThermo' instead of ' kappa -> fluidThermo'.
|
|
March 14, 2014, 04:04 |
|
#8 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
Could you please answer that last question??
|
|
March 14, 2014, 05:13 |
|
#9 |
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
In my OF 2.2.2 installation the T files of the multiRegionHeater tutorial are as follows:
heater (solid region): Code:
T { internalField uniform 300; boundaryField { ".*" { type zeroGradient; value uniform 300; } "heater_to_.*" { type compressible::turbulentTemperatureCoupledBaffleMixed; neighbourFieldName T; kappa solidThermo; kappaName none; value uniform 300; } minY { type fixedValue; value uniform 500; } } Code:
T { internalField uniform 300; boundaryField { ".*" { type zeroGradient; } "bottomAir_to_.*" { type compressible::turbulentTemperatureCoupledBaffleMixed; neighbourFieldName T; kappa fluidThermo; kappaName none; value uniform 300; } } |
|
March 14, 2014, 06:38 |
|
#10 |
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 |
This was fruitful discussion. thanks again and see you around!!
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
How can I implement temperature jump boundary condition in microchannel walls? | sima | FLUENT | 7 | January 6, 2021 21:36 |
Domain Imbalance | HMR | CFX | 5 | October 10, 2016 05:57 |
conjugate boundary condition | Daniel_Khazaei | OpenFOAM Programming & Development | 0 | December 31, 2013 13:11 |
Temperature dependant mixed Boundary condition | argonaut | OpenFOAM Pre-Processing | 2 | February 15, 2011 11:02 |
How can I implement temperature jump boundary condition in microchannel walls? | sima | FLUENT | 1 | December 8, 2010 08:20 |