not outflow at outlet in interFoam
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 |
Quote:
I would suggest you use zeroGradient for the outlet of alpha1. |
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::printStack(Foam::Ostream&) in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/trauth/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so" #2 in "/lib64/libc.so.6" #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 |
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. |
Can you post a little pic about the geometry?
Bye. |
1 Attachment(s)
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] |
Quote:
Quote:
How does your initialisation of alpha1 look like? |
Quote:
0/alpha1, in this case OF crashes after 1.78 sec. right and left are the sidewalls above inlet and outlet. Code:
FoamFile Code:
FoamFile |
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. |
Hello Santiago,
Here my 0/U: I guess pressureInletOutletVelocity equates almost to inletOutlet. Code:
FoamFile Code:
FoamFile Do you mean the boundaray-file with initialization?: Code:
FoamFile 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 |
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. |
Hi,
I forgot to give aplha1 in setFields a value, I neglected it before (thanks to Sega;)). My geometry is now half filled with water at time 0. InterFoam runs. Quote:
I took the BC from the damBreak tutorial. I think at least here, correct BC should be used. Thanks, Nico |
no outflow in interFoam
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? |
using PISO instead of PIMPLE solved the problem
|
2 Attachment(s)
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.
|
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 |
All times are GMT -4. The time now is 19:54. |