|
[Sponsors] |
May 8, 2013, 13:27 |
compressible low speed channel flow
|
#1 |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Hi all
I am trying to simulate the low Reynolds (say Re=5) mass driven compressible flow in a rectangular microchannel. I used rhoCentralFoam with the following BC: Pressure: inlet { type zeroGradient; } outlet { type fixedValue; value uniform 101315; } Velocity: inlet { type fixedValue; value uniform (0.79473 0 0); } outlet { type zeroGradient; } However, the results are not physical for example a reverse flow appears at the inlet! I am wondering if I should use another solver or other BC? Is there anyone who can help me? Thanks. |
|
May 9, 2013, 01:25 |
|
#2 |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Hi
I am really confused with the simple problem of straight rectangular channel. I need to solve the flow but really cant find out what the problem is with the setting of the openFoam. I would be greatly thankful if any body has a promising feedback. |
|
May 9, 2013, 02:26 |
|
#3 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
Dear Ali
@ inlet, fixed your pressure and @ outlet, assign a zeroGradient
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
May 9, 2013, 04:54 |
|
#4 |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
The problem in your case is that the pressure gradient in your domain is too small. You should work with a solver using a "relative pressure".
Your case reminds me this topic: http://www.cfd-online.com/Forums/ope...on-fluent.html You can also try another solver. rhoSimplecFoam / rhoPimpleFoam Edit: put your full case here. Maybe your problem is not located in the boundary conidtion. |
|
May 9, 2013, 05:35 |
|
#5 |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Dear Nima
Thanks a lot for your kind reply. I changed the BC as you said but the solution is wrong again. I also set the inlet pressure somewhat higher that the interior to avoid any back flow but surprisingly this leads to a stronger reverse flow. can you please help me on this? |
|
May 9, 2013, 05:54 |
|
#6 |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
By the way, why do you need a compressible flow ?
And try to post your full case. Maybe you made a mistake somewhere else. |
|
May 9, 2013, 06:03 |
|
#7 |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Dear Frédéric
Thanks for your comment. It really make scene and I think OF has some problem in solving the pressure field. Actually, I am new with OF and so I supposed rhoSimplecFoam / rhoPimpleFoam are for turbulent flow and cannot be used for low speed laminar cases. My case is a compressible flow throw a microchannel at Re~1. Here are the details of my mesh and BC and solver settings. It is a great help to me if you can show me the way. Many many Thanks. blockMeshDict: [QUOTE][] /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object blockMeshDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // convertToMeters 5e-5; vertices ( (0 0 0) (10 0 0) (10 1 0) (0 1 0) (0 0 1) (10 0 1) (10 1 1) (0 1 1) ); blocks ( hex (0 1 2 3 4 5 6 7) (151 51 1) simpleGrading (1 1 1) // (141 51 51) simpleGrading (3292 0.047 0.047) ); edges ( ); boundary ( inlet { type patch; faces ( (0 3 7 4) ); } outlet { type patch; faces ( (1 5 6 2) ); } bottom { type symmetryPlane; faces ( (0 4 5 1) ); } top { type patch; faces ( (3 7 6 2) ); } front_back { type empty; faces ( (0 1 2 3) (4 7 6 5) ); } ); mergePatchPairs ( ); // ************************************************** *********************** //] thermoPhysicalProperties: [QUOTE][ /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object thermophysicalProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>; mixture { specie { nMoles 1; molWeight 28.96; } thermodynamics { Cp 1007; Hf 0; } transport { mu 1.846e-05; Pr 0.711; } } // ************************************************** *********************** //] turbulenceProperties: [QUOTE][ /*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object turbulenceProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // simulationType laminar; // ************************************************** *********************** //] Pressure BC: [QUOTE][/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 101315; boundaryField { inlet { type fixedValue; value uniform 111315; } outlet { type zeroGradient; } bottom { type symmetryPlane; } top { type zeroGradient; } front_back { type empty; } } // ************************************************** *********************** //] Temperature BC: [QUOTE][//*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 300; boundaryField { inlet { type fixedValue; value uniform 300; } outlet { type zeroGradient; } bottom { type symmetryPlane; } top { type fixedValue; value uniform 350; } front_back { type empty; } } // ************************************************** *********************** //] Velocity BC: [QUOTE][/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.0.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0.79473 0 0); boundaryField { inlet { type fixedValue; value uniform (0.79473 0 0); } outlet { type zeroGradient; } bottom { type symmetryPlane; } top { type fixedValue; value uniform (0 0 0); } front_back { type empty; } } // ************************************************** *********************** //] controlDict: [QUOTE][/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application rhoCentralFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 1e-02; deltaT 1e-6; writeControl adjustableRunTime; writeInterval 1e-5; cycleWrite 0; writeFormat ascii; writePrecision 10; writeCompression off; timeFormat general; timePrecision 6; adjustTimeStep yes; maxCo 0.2; maxDeltaT 1; // ************************************************** *********************** //] fvSchemes: [QUOTE][/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // fluxScheme Kurganov; //fluxScheme Tadmor; ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(tauMC) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; reconstruct(rho) vanLeer; reconstruct(U) vanLeerV; reconstruct(T) vanLeer; //reconstruct(rho) upwind; //reconstruct(U) upwind; //reconstruct(T) upwind; } snGradSchemes { default corrected; } // ************************************************** *********************** //] fv solution: [QUOTE][/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "(rho|rhoU|rhoE)" { solver diagonal; } U //"(U|e)" { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-09; relTol 0.01; } e { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-10 relTol 0; } h { $U; tolerance 1e-10; relTol 0; } } // ************************************************** *********************** //] |
|
May 9, 2013, 06:11 |
|
#8 | |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
Instead of copying all the file here, you can actually upload them. There is a function "Attach Files" just below the submit button.
rhoSimplecFoam can be either turbulent or laminar. You can use k-epsilon, k-omega, Sparlat Allmaras, or laminar. And if you use rhoPimpleFoam, you can use all those model and even LES. The official description is: Quote:
|
||
May 9, 2013, 06:15 |
|
#9 |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
I'm not familiar with rhoCentralFoam but I don't think it is suitable for you. rhoCentralFoam is a density based solver (which was primarily designed for supersonic flow) while rhoSimplecFoam is a pressure based solver (which was primarily designed for subsonic flow).
|
|
May 9, 2013, 06:17 |
|
#10 | |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Quote:
I have solved the flow with an incompressible CFD code but whereas the pressure drop in microchannels are considerable and also there is a considerable temperature gradient in my problem, I am curious to see what happen if I use a compressible solver. Actually I have to compare my results with those of compressible case. |
||
May 9, 2013, 06:29 |
|
#11 |
New Member
Ali
Join Date: May 2013
Posts: 9
Rep Power: 13 |
Thanks for you comments dear Frédéric
(I am a row new member in this site )OK; I will try the rhoSimplecFoam hope it work. Then I will tell you about the results. Again thanks for your kind informative comments. |
|
May 9, 2013, 08:40 |
|
#12 | |
Senior Member
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 249
Rep Power: 17 |
Quote:
Also, are you sure your flow is really 100% laminar ? How is the flow at the inlet of your simulation ? Does it come from a "tube", how long ? If yes, you might need to consider the turbulence of the upstream flow. The problem in micro channel, if I remember well, is that the boundary layers tend to meet at the middle of the channel. Maybe a fine mesh with a k-omega SST model can handle this problem. You might need to compare two simulations (laminar vs k-omega sst). |
||
Tags |
channel flow, compressible solver, low speed, mass driven, rhocentralfoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Low Mach number Compressible jet flow using LES | ankgupta8um | OpenFOAM Running, Solving & CFD | 7 | January 15, 2011 14:38 |
Can 'shock waves' occur in viscous fluid flows? | diaw | Main CFD Forum | 104 | February 16, 2006 06:44 |
Compressible Flow Modelling? | yeo | FLUENT | 4 | March 7, 2003 08:08 |
compressible channel flow | sky | Main CFD Forum | 0 | December 5, 2002 10:05 |
compressible channel flow.. | R.D.Prabhu | Main CFD Forum | 0 | July 17, 1998 18:23 |