|
[Sponsors] |
![]() |
![]() |
#1 |
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
Hi,
I've a simple square geometry with a irregular (up-and down) bottom. BC are inlet, outlet, top-atmosphere and walls in interFoam laminar. The model runs but not with my expected results. The problem is, that there's no outflow at the outlet. Looks like a closed wall, liquid (aplha1) is bouncing backwards. checkMesh is OK. My BC: p_rgh: inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } U: inlet { type fixedValue; value uniform (0.5 0 0); } outlet { type zeroGradient; } alpha1: inlet { type fixedValue; value uniform 1; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } Thanks for help, Nico |
|
![]() |
![]() |
![]() |
![]() |
#2 | |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 21 ![]() |
Quote:
I would suggest you use zeroGradient for the outlet of alpha1.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
||
![]() |
![]() |
![]() |
![]() |
#3 |
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
Thanks for your answer,
setting alpha1 on zeroGradient was my step before. The model runs only 1-2 seconds and this error message occurs: MULES: Solving for alpha1 #0 Foam::error: ![]() #3 void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libfiniteVolume.so" #4 void Foam::MULES::explicitSolve<Foam::geometricOneField , Foam::zeroField, Foam::zeroField>(Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::zeroField const&, Foam::zeroField const&, double, double) in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libfiniteVolume.so" #5 Foam::MULES::explicitSolve(Foam::GeometricField<do uble, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, double, double) in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libfiniteVolume.so" #6 in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/interFoam" #7 __libc_start_main in "/lib64/libc.so.6" #8 at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116 Gleitkomma-Ausnahme Any idea what could be the reason? Thanks |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 21 ![]() |
Hm, this is strange indeed.
It concerns the MULES solver for solving the VOF-equation. I would suggest you to re-check everything converning alpha1 including boundaries and initial condition.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|
![]() |
![]() |
![]() |
![]() |
#5 |
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24 ![]() |
Can you post a little pic about the geometry?
Bye.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
Here's my geometry.
- Inlet on the left, outlet on the right side, both bc are only in the lower part of the sidewalls. - The top boundary is set as atmosphere. - Bottom, front, and backside are walls. The Mesh is coarse, maybe refinement would lead to better results?! Thanks for your help. Nico [IMG]file:///home/trauth/Dokumente/Graphics/geo.jpg[/IMG] |
|
![]() |
![]() |
![]() |
![]() |
#7 | ||
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 21 ![]() |
Quote:
Quote:
How does your initialisation of alpha1 look like?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" |
|||
![]() |
![]() |
![]() |
![]() |
#8 |
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
I've defined boundaries in blender and engrid before.
0/alpha1, in this case OF crashes after 1.78 sec. right and left are the sidewalls above inlet and outlet. Code:
FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object alpha1; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0; boundaryField { right { type zeroGradient; } inlet { type fixedValue; value uniform 1; } outlet { type zeroGradient; } front { type zeroGradient; } back { type zeroGradient; } top { type inletOutlet; inletValue uniform 0; value uniform 0; } bottom { type zeroGradient; } left { type zeroGradient; } } Code:
FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object alpha1; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0; boundaryField { right { type zeroGradient; } inlet { type fixedValue; value uniform 1; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } front { type zeroGradient; } back { type zeroGradient; } top { type inletOutlet; inletValue uniform 0; value uniform 0; } bottom { type zeroGradient; } left { type zeroGradient; } } |
|
![]() |
![]() |
![]() |
![]() |
#9 | |
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24 ![]() |
Hello Nico, first settings appear to be correct, except for:
Quote:
A little shortcut to start with this problem is to put a wall on the top (atmosphere) and to use inletOutlet in the top part of the inlet to ensure air entrance. Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar |
||
![]() |
![]() |
![]() |
![]() |
#10 | ||
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
Hello Santiago,
Here my 0/U: I guess pressureInletOutletVelocity equates almost to inletOutlet. Code:
FoamFile { version 2.0; format binary; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { right { type fixedValue; value uniform (0 0 0); } inlet { type fixedValue; value uniform (0.5 0 0); } outlet { type zeroGradient; } front { type fixedValue; value uniform (0 0 0); } back { type fixedValue; value uniform (0 0 0); } top { type inletOutlet; inletValue uniform (0 0 0); value uniform (0 0 0); //before: //type pressureInletOutletVelocity; //value uniform (0 0 0); } bottom { type fixedValue; value uniform (0 0 0); } left { type fixedValue; value uniform (0 0 0); } } Code:
FoamFile { version 2.0; format binary; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 0; boundaryField { right { type buoyantPressure; value uniform 0; } inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } front { type buoyantPressure; value uniform 0; } back { type buoyantPressure; value uniform 0; } top { type totalPressure; p0 uniform 0; U U; phi phi; rho rho; psi none; gamma 1; value uniform 0; } bottom { type buoyantPressure; value uniform 0; } left { type buoyantPressure; value uniform 0; } } Do you mean the boundaray-file with initialization?: Code:
FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 8 ( right { type wall; nFaces 29; startFace 11746; } inlet { type patch; nFaces 26; startFace 11775; } outlet { type patch; nFaces 26; startFace 11801; } front { type wall; nFaces 879; startFace 11827; } back { type wall; nFaces 907; startFace 12706; } top { type patch; nFaces 482; startFace 13613; } bottom { type wall; nFaces 478; startFace 14095; } left { type wall; nFaces 33; startFace 14573; } ) Quote:
aplha1: inletOutlet into zeroGradient U: pressureInletOutletVelocity into type inletOutlet; inletValue uniform (0 0 0); value uniform (0 0 0); interFoam runs only 1.3 seconds. Quote:
Thanks for help. Regards, Nico |
|||
![]() |
![]() |
![]() |
![]() |
#11 |
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24 ![]() |
Nico, your settings appear to be OK, I only would change (as you already did) the bouyantPressure BC by zeroGradient. Pressure equation is Poisson-like, therefore zeroGradient is the correct BC for walls. I would use these settings with a very small timestep, i.e. 1e-7, and then would increase it until run explodes.
Try this, if you continue having problems, please post the output. Good luck.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar |
|
![]() |
![]() |
![]() |
![]() |
#12 | |
Member
Nico T
Join Date: Aug 2010
Location: Leipzig, Germany
Posts: 39
Rep Power: 16 ![]() |
Hi,
I forgot to give aplha1 in setFields a value, I neglected it before (thanks to Sega ![]() Quote:
I took the BC from the damBreak tutorial. I think at least here, correct BC should be used. Thanks, Nico |
||
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 242
Rep Power: 17 ![]() |
dear FOAMERS,
I used type inletOutlet; inletValue uniform (0 0 0); for U at the outlet and type zeroGradient; for alpha1 at the outlet and tried aswell type inletOutlet; inletValue uniform 0; for alpha1, and all these settings work fine with OF 1.7.1 but create no outflow at OF 2.1.x., so maybe there is some change between the versions? |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 242
Rep Power: 17 ![]() |
using PISO instead of PIMPLE solved the problem
|
|
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 242
Rep Power: 17 ![]() |
Ok turning old searching the cause of alpha1 being reflected at the outflow, I finally got it (ints not about PISO and PIMPLE). Maybe this is a bug dependent on ubuntu version, but it is quite relevant. The difference between the two pictures below showing an outflow of a channel is only that I moved the grid from positive x quadrant to negative x quadrant. When the whole grid lies at a position that the x-coordinates are smaller than 0 the outflow works! If using zeroGradient for p_rgh at the outflow, it works aswell fine for a grid with positive x coordinates. Anyway, I would be happy for any explanation on this.
Last edited by vonboett; June 14, 2012 at 09:06. |
|
![]() |
![]() |
![]() |
![]() |
#16 |
New Member
Bahram Haddadi
Join Date: Feb 2014
Location: Vienna, Austria
Posts: 20
Rep Power: 13 ![]() |
Dear Albrecht,
Since this is more than 10 years from your post here and the problem still exists in the new versions of OpenFOAM, I'll prepare a bog report and submit it to the OpenFOAM. Best regrads |
|
![]() |
![]() |
![]() |
Thread Tools | Search this Thread |
Display Modes | |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Using interFoam, phase piles up at pipe outlet | kjetil | OpenFOAM Running, Solving & CFD | 4 | August 24, 2010 03:18 |
Outlet boundary setup for interFoam | mittal | OpenFOAM Running, Solving & CFD | 2 | July 14, 2010 08:59 |
B.C.S on outflow outlet and pressure outlet | kenneth | Main CFD Forum | 4 | May 29, 2008 20:57 |
HELP !!difference of outflow and pressure outlet?? | Kwong | FLUENT | 1 | April 11, 2007 05:04 |
VOF Outlet boundary condition in cfd - ace | JM | Main CFD Forum | 0 | December 15, 2006 08:07 |