Slow convergence of chtMultiRegionSimpleFoam

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

September 29, 2010, 13:21
Slow convergence of chtMultiRegionSimpleFoam
#1
New Member

Charles McCreary
Join Date: Jun 2010
Posts: 9
Rep Power: 7
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.

Update:

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
 poc.tar.gz (5.3 KB, 28 views) frame_against_ceiling.tar.gz (9.1 KB, 20 views)

Last edited by crmccreary; October 5, 2010 at 11:32. Reason: update

 November 11, 2010, 21:52 #2 New Member   Charles McCreary Join Date: Jun 2010 Posts: 9 Rep Power: 7 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://github.com/crmccreary/chtMultiRegionSimpleFoam-example.git as well as the sample problem git://github.com/crmccreary/chtMultiRegionSimpleFoam-example.git

 Tags chtmultiregionsimplefoam, flux

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post nasdak CFX 2 June 29, 2009 01:17 pad STAR-CCM+ 2 May 27, 2009 05:17 demigod FLUENT 1 October 5, 2005 08:03 Biga Main CFD Forum 2 November 18, 2004 17:51 Jesper CFX 1 July 7, 2004 16:59

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