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

OpenFOAM Version 5 vs 6 with respect to chtMultiRegionFoam

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2019, 01:36
Default OpenFOAM Version 5 vs 6 with respect to chtMultiRegionFoam
  #1
Member
 
Adam
Join Date: Nov 2018
Posts: 36
Rep Power: 8
Adam_K is on a distinguished road
I've been having an issue with multiPhase heat transfer in solid (see this thread) and now I'm wondering if it's an issue with the version of OpenFOAM.


In the v5 user guide it says:

Quote:
chtMultiRegionFoam

Transient solver for buoyant, turbulent fluid flow and solid heat conduction with conjugate heat transfer between solid and fluid regions.
While in the v6 user guide it says :

Quote:
chtMultiRegionFoam

Solver for steady or transient fluid flow and solid heat conduction, with conjugate heat transfer between regions, buoyancy effects, turbulence, reactions and radiation modelling.
Based on the wording, I'm left to wonder if they mean that v5 can only handle heat transfer between solid AND fluid regions, but not between two solid regions.

Does this mean that I need to be using OpenFOAM v6 in order to look at heat transfer across solid-solid interfaces (with and without thermal resistances)?
Adam_K is offline   Reply With Quote

Old   February 27, 2019, 14:23
Default
  #2
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 11
Robin.Kamenicky is on a distinguished road
Hi Adam,

I have had a quick look at the solvers. I think that both of them are capable to deal with solid-solid interface. multiRegionHeater tutorial in of-5 calculates solid-solid interface.

I have checked a bit the codes. I have not noticed any crucial difference for solid-solid interface.

In my opinion, the type of the interface is only dealt by BC. Which do you use? I have not had a look at your case setup.

Kind regards,
Robin
Robin.Kamenicky is offline   Reply With Quote

Old   February 28, 2019, 01:36
Default
  #3
Member
 
Adam
Join Date: Nov 2018
Posts: 36
Rep Power: 8
Adam_K is on a distinguished road
Quote:
Originally Posted by Robin.Kamenicky View Post
Hi Adam,

I have had a quick look at the solvers. I think that both of them are capable to deal with solid-solid interface. multiRegionHeater tutorial in of-5 calculates solid-solid interface.

I have checked a bit the codes. I have not noticed any crucial difference for solid-solid interface.

In my opinion, the type of the interface is only dealt by BC. Which do you use? I have not had a look at your case setup.

Kind regards,
Robin
Thanks for taking a look at the solvers. I was looking at them as well, but am not sure that I'd be able to really identify the differences.

I have been following the multiRegionHeater tutorial to see how to set up my case. I have defined in 0/matrix/T
Code:
boundaryField
{
    matrix_to_fibres
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
        kappaMethod     solidThermo;
    }
...
}
0/fibres/T includes
Code:
boundaryField
{
    fibres_to_matrix
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 300;
        Tnbr            T;
        kappaMethod     solidThermo;
    }
...
}
The code runs, it just seems as if there's barely any exchange between the two phases. For example inclusions of the same thermal diffusivity leads to an overall temperature response (as measured by the increase in temperature at the center of the slab) much slower than expected, 5% of a material with K = 30 mixed into a matrix of K = 300 should not respond as if the K were somewhere around 3.

If I add the following lines, I get an exchange between the two phases. However, they do not tend towards a reasonable limiting case, I describe a few of my results in this thread.
Code:
        thicknessLayers	(1e-2);
        kappaLayers	    (1);
Adam_K is offline   Reply With Quote

Old   March 2, 2019, 11:47
Default
  #4
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 11
Robin.Kamenicky is on a distinguished road
Hi Adam,

I have answered you in the other thread.

It is good to notice that the BC just evaluates the temperature for given region.
If you define layer thickness then it uses:
Code:
contactRes = thicknessLayers/kappaLayers
contactRes = 1.0/contactRes
nbrKDelta = contactRes
if you do not use it
Code:
nbrKDelta = kappa_nbrField*distance_cells_on_both_sides
Then the code is common for both cases. It calculates
Code:
valueFracion = nbrKDelta/(nbrKDelta+myKDelta)
Then it just estimate temperature based on the valueFraction.

I have a few ideas, what could be the problem but I need the log file or possibly try to run it myself. Hope this helps somehow.

Kind regards,
Robin
Robin.Kamenicky is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
simpleFoam convergence issue Harnoor OpenFOAM Running, Solving & CFD 13 November 16, 2016 09:23
OpenFOAM Foundation Releases OpenFOAMŪ Version 2.1.1 opencfd OpenFOAM Announcements from ESI-OpenCFD 0 May 31, 2012 10:07
OpenFOAM Version 1.6 Released opencfd OpenFOAM Announcements from ESI-OpenCFD 0 July 27, 2009 18:55
OpenFOAM Version 1.4 Released OpenFOAM discussion board administrator OpenFOAM Announcements from ESI-OpenCFD 0 April 11, 2007 19:56
OpenFOAM Version 1.1 Released OpenFOAM discussion board administrator OpenFOAM Announcements from ESI-OpenCFD 0 March 11, 2005 06:33


All times are GMT -4. The time now is 16:54.