CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Question about temperature boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 12, 2014, 06:25
Default Question about temperature boundary condition
  #1
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
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;
    }
}
vasava is offline   Reply With Quote

Old   March 12, 2014, 11:38
Default
  #2
New Member
 
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 4
akrasemann is on a distinguished road
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.
akrasemann is offline   Reply With Quote

Old   March 13, 2014, 09:29
Default
  #3
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
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.
vasava is offline   Reply With Quote

Old   March 13, 2014, 09:55
Default
  #4
New Member
 
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 4
akrasemann is on a distinguished road
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?
akrasemann is offline   Reply With Quote

Old   March 14, 2014, 03:39
Default
  #5
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
Thank you for your comments.

Quote:
Originally Posted by akrasemann View Post
How do you get 3 regions?
Sorry i described mesh generation for some other case. I have 2 regions one fluid and one is pipe.

Quote:
Originally Posted by akrasemann View Post
So can you explain in detail, what exactly your problem is?
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.
vasava is offline   Reply With Quote

Old   March 14, 2014, 03:52
Default
  #6
New Member
 
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 4
akrasemann is on a distinguished road
You are welcome
akrasemann is offline   Reply With Quote

Old   March 14, 2014, 03:53
Default
  #7
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
Quote:
Originally Posted by akrasemann View Post
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.
I copied that condition from tutorial 'multiRegionHeater' and 'multiRegionLiquidHeater'. Could you please elaborate on the reason for using ' kappa -> solidThermo' instead of ' kappa -> fluidThermo'.
vasava is offline   Reply With Quote

Old   March 14, 2014, 05:04
Default
  #8
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
Could you please answer that last question??
vasava is offline   Reply With Quote

Old   March 14, 2014, 06:13
Default
  #9
New Member
 
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 4
akrasemann is on a distinguished road
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;
            }
        }
whereas for bottomAir (fluid region)
Code:
    T
    {
        internalField   uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
            }

            "bottomAir_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           fluidThermo;
                kappaName       none;
                value           uniform 300;
            }
        }
which sounds reasonable to me, as ones specifies the thermal conductivity (kappa) of the active region.
akrasemann is offline   Reply With Quote

Old   March 14, 2014, 07:38
Default
  #10
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
This was fruitful discussion. thanks again and see you around!!
vasava 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
Domain Imbalance HMR CFX 5 October 10, 2016 05:57
How can I implement temperature jump boundary condition in microchannel walls? sima FLUENT 6 May 18, 2016 21:50
conjugate boundary condition Daniel_Khazaei OpenFOAM Programming & Development 0 December 31, 2013 14:11
Temperature dependant mixed Boundary condition argonaut OpenFOAM Pre-Processing 2 February 15, 2011 12:02
How can I implement temperature jump boundary condition in microchannel walls? sima FLUENT 1 December 8, 2010 09:20


All times are GMT -4. The time now is 19:13.