CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM

Slow convergence of chtMultiRegionSimpleFoam

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

LinkBack Thread Tools Display Modes
Old   September 29, 2010, 13:21
Default Slow convergence of chtMultiRegionSimpleFoam
New Member
Charles McCreary
Join Date: Jun 2010
Posts: 9
Rep Power: 7
crmccreary is on a distinguished road
I have a rather simple chtMultiRegionSimpleFoam problem that I am using to verify and validate a natural convection simulation. Unlike the chtMultiRegionSimpleFoam tutorial, I have applied a fixed gradient bc of q/k instead of a fixed temperature. I would expect that the solid would heat up much quicker than it does. Instead, the temperature rises very slowly and is still nowhere near the back-of-the-envelope calculation after a time of 10000.

I've attached the case, in case someone would like to see what the problem is.


Although, I've given up hope for the cht solver working with all flux inputs, I can obtain the desired solution iteratively by applying a temperature and monitoring the flux at the interfacial boundary by setting the debug flag

solidWallHeatFluxTemperatureFvPatchScalarField 2;

in the master or home (~/.OpenFOAM/1.7.0/controlDict) controlDict.

I am attaching a case in which I model the aluminum frame of a thin LED light fixture nearly flush against the ceiling. To generate the mesh, I have a written a small python program to generate the blockMeshDict file.

Update 2:

From inspection of the coupling patch code, it appears that only the calculated wall temperature is exchanged. Thus if I start the solid at 300 deg and the fluid at 300 deg, the wall temperature will be 300 deg. Considering that q = delta_T/R_tot where R_tot is the thermal resistance, the expected delta_T will be very small.

If instead of sharing the wall temperature, we instead calculate the flux at the interface and apply a fixed gradient to the solid and the harmonic mean of Ts, Tf to the wall for the fluid, then the initial fixed gradient will be zero (adiabatic). In this way, I think the temperature convergence problem can be solved when applying only a directGradient to the solid. I will be pursuing creating and/or funding such a boundary condition. A cursory literature search has indicated that this has been done before in OpenFOAM. I will start with compressible::turbulentTemperatureCoupledBaffle and extend from there.

In the interim, I have found that I can iterate a few times with applied temperature while monitoring the interfacial wall flux to determine the applied temperature that produces the desired flux. Not optimum, but workable.
Attached Files
File Type: gz poc.tar.gz (5.3 KB, 28 views)
File Type: gz frame_against_ceiling.tar.gz (9.1 KB, 20 views)

Last edited by crmccreary; October 5, 2010 at 11:32. Reason: update
crmccreary is offline   Reply With Quote

Old   November 11, 2010, 21:52
New Member
Charles McCreary
Join Date: Jun 2010
Posts: 9
Rep Power: 7
crmccreary is on a distinguished road
Update 3:
The solution was in OpenFOAM I think since 1.6.
Steps for a chtMultiRegionSimpleFoam solution:
1.) Apply the heatFlux with solidWallHeatFluxTemperature
2.) Couple the fluid and solid with solidWallMixedTemperatureCoupled. This requires copying and modfying the solidWallMixedTemperatureCoupled in applications/solvers/heatTransfer/chtMultiRegionFoam/derivedFvPatchFields/solidWallMixedTemperatureCoupled to applications/solvers/heatTransfer/chtMultiRegionSimpleFoam/derivedFvPatchFields/solidWallMixedTemperatureCoupled
3.) Make changes to the solid solution similar to this post

I have pushed a git branch of OpenFOAM 1.7.x to git:// as well as the sample problem git://
crmccreary is offline   Reply With Quote


chtmultiregionsimplefoam, flux

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
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
Slow convergence using stagnation inlet pad STAR-CCM+ 2 May 27, 2009 05:17
Ultra slow convergence velocity in the simulation demigod FLUENT 1 October 5, 2005 08:03
Slow convergence for Boundary Layer flow Biga Main CFD Forum 2 November 18, 2004 17:51
Slow convergence Jesper CFX 1 July 7, 2004 16:59

All times are GMT -4. The time now is 19:53.