|
[Sponsors] |
May 1, 2020, 11:46 |
chtMultiregionFoam issues with heat sources
|
#1 |
New Member
Nicolò Badodi
Join Date: Mar 2020
Posts: 20
Rep Power: 6 |
Hi everyone!
I'm in desperate need of help! I set up a case in which a cylindrical heating element 2 cm in diameter and 4 cm long is heated with a power of 404 W and irradiates the surroundings. The heater is surrounded by vacuum (modeled as air with very low kappa and cp, frozen flow), and everything is enclosed in a reradiating furnace wall, except that two stripes of this wall are actually held at 600K and so absorb all the exceding heat. I used fvDOM as radiation model. The analytical calculation shows that the heater, which is made of silicon carbide, should heat up at a rate of 52 K/s, while calculation with cht shows a heating of only 8K/s, which is much lower. The setup can be seen in the image I attached (PS there is a mesh in between the heater and the external wall) I'll post here the configuration files related to the heating element: Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 7 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant/heater"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // heatSource { type scalarSemiImplicitSource; active true; scalarSemiImplicitSourceCoeffs { selectionMode all; volumeMode absolute; //specific;//absolute; injectionRateSuSp { rho (3200 0); //TODO: is this required? h (404 0); //TODO: 404 W is this the right unit? } } } //************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 7 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant/solid"; object thermophysicalProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; //sensibleEnthalpy; } mixture { // Silicon carbide specie { molWeight 1000; } equationOfState { rho 3200;//3200; //g/cm2 } transport { kappa 120;//120; //W/cm*K } thermodynamics { Hf 0; Cp 190; //J/(g*K) } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 7 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0/solid"; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 0 0 1 0 0 0 ]; internalField uniform 300; boundaryField { #includeEtc "caseDicts/setConstraintTypes" front_cyc { type cyclic; } back_cyc { type cyclic; } heater_to_air { type compressible::turbulentTemperatureRadCoupledMixed; value uniform 300; Tnbr T; T T; kappaMethod solidThermo; qrNbr qr; qr none; /* type zeroGradient;*/ } } // ************************************************************************* // the whole case can be found here: https://drive.google.com/open?id=1xi...5dn-LkhGKw7QKl Any idea of what could be causing this issue? Wrong unit in the thermophysical properties? Wrong injection of heat? Please help! |
|
May 14, 2020, 04:00 |
|
#2 |
Senior Member
Carlos Rubio Abujas
Join Date: Jan 2018
Location: Spain
Posts: 127
Rep Power: 11 |
Hi Nicoló,
I think the heatSource may have different units. The field h is defined inside the source code as solidThermo::he, which have units of [J/kg]. So the rate of change may be [W/kg] if the volumeMode is absolute, as it seems your case. If that is correct and you want the cylinder to provide 404W, you need to set the scalarSemiImplicitSource to be around 5050 W/kg (according to some rough calculations). That is in the order of the error you mentioned, so may be reasonable to try. Hopes it helps! |
|
June 13, 2020, 06:16 |
|
#3 |
New Member
Nicolò Badodi
Join Date: Mar 2020
Posts: 20
Rep Power: 6 |
Hi Crubio!
Turns out that the units were right, but there was an error in the fvSolution file, that was making my solver use the PGC algorithm for the solution of the enthalpy equation instead of GAMG. All solved now! |
|
Tags |
cfd, chtmulitregionfoam, heat and mass transfer, heat sources, multi region |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Two simultaneous heat sources in ANSYS APDL | Unkinunki | ANSYS | 10 | May 24, 2021 08:47 |
OpenFOAM heat sink chtMultiRegionFoam | amdk136 | OpenFOAM Running, Solving & CFD | 1 | September 21, 2020 08:07 |
chtMultiRegionFoam connection between solid and fluid region of heat exchanger | ahab | OpenFOAM | 1 | December 18, 2019 01:37 |
Domain Reference Pressure and mass flow inlet boundary | AdidaKK | CFX | 75 | August 20, 2018 06:37 |
Convective Heat Transfer - Heat Exchanger | Mark | CFX | 6 | November 15, 2004 16:55 |