# Heat transfer convergence problem

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 31, 2014, 05:44 Heat transfer convergence problem #1 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 I'm trying to simulate a problem which involves heat transfer from a very hot gas (plasma) in a wall. Concerning this problem, my solver is basically a merged version of sonicFoam and chtMultiRegionFoam (only the heat transfer part). The plasma has a large radiative flux and the wall isn't a very good heat conductor, so melting and evaporation occurs in reality. I'm using the compressible::turbulentTemperatureRadCoupledMixed boundary condition that considers heat conduction and radiative heat fluxes through the boundary. This boundary condition always results in a temperature at the patch of 0 K... I've tried various things, increasing iterations and using relaxation factors but without success. The temperature will start with a negative (!) value at the patch in the iteration procedure and converge against 0 K in a few steps. The alpha value in the code of the BC will start oscillating with an increasing amplitude. Using the compressible::turbulentTemperatureCoupledBaffleMix ed BC, the solution will converge, but since the radiation isn't considered this BC is not applicable to my problem. I would expect the total heat fluxes to be the same on both sides of the patch when converged to satisfy energy conservation. Any ideas for this? You can also take a look at my related topic here: http://www.cfd-online.com/Forums/ope...pling-bcs.html Ramzy1990 likes this.

 November 3, 2014, 05:17 #2 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 I tracked it down to a numerical problem. I wrote the convergence series as a script in Matlab, so I could play with the parameters and see when I get a converging solution. Due to the high temperatures in a plasma, there is a very large radiative heat flux (on the order of 1e9 W/m²). Using lower heat fluxes leads to a converging solution, and using smaller cells also converges. However, the cells are already extremely low at the boundary (about 5e-7m), so this will lead to massive performance impacts if I need this cell size. I also tried underrelaxing, but it doesn't have any (positive) influence on the convergence behavior. I'm not quite sure yet where exactly the problem comes from, can anyone think of an alternative formulation that might give less numerical problems and converge better? For reference, here's the Matlab script with example data: Code: n = 20; T0=15000; Tf0=[293]; Tf1=[293]; T1=293; kappa0 = 0.05; kappa1 = 0.4; delta0 = 1/2e6/4; delta1 = 1/2.85714e+06/4; Qr0 = 2.99454e9; Qr1 = 0; K0 = kappa0/delta0; K1 = kappa1/delta1; QrT0 = [0]; QrT1 = [0]; sum0 = [1]; sum1 = [1]; den0 = [1]; den1 = [1]; relax = 1; for i=2:n QrT0(i) = (Qr0 + Qr1)/Tf0(i-1); QrT1(i) = (Qr0 + Qr1)/Tf1(i-1); den0(i) = K0-QrT0(i)+K1; den1(i) = K0-QrT1(i)+K1; Tf0(i) = relax * K1/(K0-QrT0(i)+K1) * T1 + K0/(K0-QrT0(i)+K1) * T0 + (1-relax) * Tf0(i-1); Tf1(i) = relax * K0/(K0-QrT1(i)+K1) * T0 + K1/(K0-QrT1(i)+K1) * T1 + (1-relax) * Tf1(i-1); sum0(i) = K0/(K0-QrT0(i)+K1) + K1/(K0-QrT0(i)+K1); sum1(i) = K0/(K0-QrT1(i)+K1) + K1/(K0-QrT1(i)+K1); end; plot(1:n, Tf0, 1:n, Tf1); % plot(1:n, den0, 1:n, den1); % plot(1:n, QrT0, 1:n, QrT1); % plot(1:n, sum0, 1:n, sum1); vscalon and Ramzy1990 like this.

 November 3, 2014, 11:05 #3 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 I now believe that this is not a numerical problem, but rather a specific convergence range of the iteration series, and there's not much one can do within this formulation. However, I found that using a nonlinear cell spacing on the wall allows me to perform this calculation with the same amount of cells and without limiting my time step size, so I'm just sacrificing some accuracy further away in the solid, which is perfectly fine for me. I'm still fighting some weird bug in the code, but it's likely fixable. Ramzy1990 likes this.

 October 14, 2023, 11:12 #4 New Member   jaehun LEE Join Date: Jan 2023 Posts: 6 Rep Power: 3 Hello, thanks for your kind explanation about Radiation B.C now I'm working on the Combusion simulation using multiRegionReactingFoam, which is modified from chtmultiRegionFoam to deal with reacting flows. in my case, the radiative heat flux is quite important, so i found compressible:turbulentemperatureradcoupledmixed Coupled B.C. but when the emissivity is big (~ 1.0), the radiative heat flux is too high, that cause the simulation diverges. (solid temperature << 70K). also, i'm testing parametric study with variation of emissivty (~ 0.01). it seems quite stable. i think you already experience this kind of problem. could you give me some advice??

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post siva0182 FLUENT 6 February 22, 2019 06:00 eng_yasser_2020 FLUENT 3 February 19, 2019 02:13 rogbrito CFX 1 January 29, 2012 17:48 Manoj Padmakarrao Raut Siemens 0 March 17, 2005 00:01 Brian CFX 0 September 13, 2004 01:19

All times are GMT -4. The time now is 03:17.

 Contact Us - CFD Online - Privacy Statement - Top