
[Sponsors] 
September 29, 2010, 13:21 
Slow convergence of chtMultiRegionSimpleFoam

#1 
New Member
Charles McCreary
Join Date: Jun 2010
Posts: 9
Rep Power: 8 
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 backoftheenvelope 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. 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: 8 
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/chtMultiRegionSimpleFoamexample.git as well as the sample problem git://github.com/crmccreary/chtMultiRegionSimpleFoamexample.git 

Tags 
chtmultiregionsimplefoam, flux 
Thread Tools  
Display Modes  


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  STARCCM+  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 