|
[Sponsors] |
March 30, 2012, 04:04 |
Outlet BC with Interfoam
|
#1 |
Senior Member
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 17 |
I'm simulating a waterfall device using Interfoam. Everything's fine but the outlet.
If you look at the picture you'll see the water at the end of the domain that seems reflected by the outlet surface. Isn't supposed to just disappear as soon as it touchs the surface ? Here is my BC: 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 { inlet { type fixedValue; value uniform 1; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } walls { type zeroGradient; } defaultFaces { type zeroGradient; } } FoamFile { version 2.0; format ascii; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type buoyantPressure; value uniform 0; } outlet { type totalPressure; p0 uniform 0; U U; phi phi; rho rho; psi none; gamma 1; value uniform 0; } walls { type buoyantPressure; value uniform 0; } defaultFaces { type buoyantPressure; value uniform 0; } } FoamFile { version 2.0; format ascii; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { outlet { type pressureInletOutletVelocity; value uniform (0 0 0); } inlet { type fixedValue; value uniform (0 1 0); } walls { type fixedValue; value uniform (0 0 0); } defaultFaces { type fixedValue; value uniform (0 0 0); } } |
|
March 30, 2012, 05:07 |
|
#2 |
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 14 |
I would rather go with zeroGradient instead of buoyantPressure for the "inlet"...
Furthermore, could you provide some more information? Such as velocities / grid and maybe schemes and solution algorithms? Do you have a laminar or turbulent case? I usually have defaultFaces set to "empty" for everything. But I do not know what "faces" are inside your defaultFaces "class"... As already mentioned, some more information would be useful for me and others to help you. |
|
March 30, 2012, 05:36 |
|
#3 |
Senior Member
Pablo Higuera
Join Date: Jan 2011
Location: Auckland
Posts: 627
Rep Power: 19 |
I think it is perfectly fine. I have used that exactly outlet condition with a standing plunging wave crossing the boundary and I did not get any reflections or disturbances.
May that water come from the first time steps when the waterfall develops? Maybe due to air movement on the first time steps the falling water may not reach so far, leading to what you see (there's a wall on the bottom, right?) |
|
March 30, 2012, 06:15 |
|
#4 |
Senior Member
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 17 |
Sorry for the lack of information.
At the moment I'm working with a sample case so laminar model only. DefaultFaces BC is there but there are no faces assigned to it (I have to remove it). The grid is quite coarse, but good for its purpose. Here is the checkmesh result: Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.1 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ /* Windows 32 and 64 bit porting by blueCAPE: http://www.bluecape.com.pt *\ | Based on Windows porting (2.0.x v4) by Symscape: http://www.symscape.com | \*---------------------------------------------------------------------------*/ Build : 2.1-c62f134541ee Exec : checkmesh Date : Mar 30 2012 Time : 12:09:17 Host : "UFFTECNICO7" PID : 2072 Case : C:/TAPS/CFD/cascmurotest nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 406885 faces: 1140167 internal faces: 1080679 cells: 367648 boundary patches: 4 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 356140 prisms: 2740 wedges: 0 pyramids: 0 tet wedges: 18 tetrahedra: 0 polyhedra: 8750 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology defaultFaces 0 0 ok (empty) inlet 262 318 ok (non-closed singly connected) outlet 48316 49856 ok (non-closed singly connected) walls 10910 11571 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-0.035 -0.03 -0.03) (0.035 0.36 0.2) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (-3.8139e-015 6.38513e-016 8.69605e-016) OK. Max cell openness = 3.55749e-016 OK. Max aspect ratio = 7.29527 OK. Minumum face area = 1.76004e-007. Maximum face area = 6.04908e-006. Face area magnitudes OK. Min volume = 9.94385e-011. Max volume = 1.2288e-008. Total volume = 0.00265921. Cell volumes OK. Mesh non-orthogonality Max: 47.0849 average: 4.61111 Non-orthogonality check OK. Face pyramids OK. Max skewness = 1.94815 OK. Coupled point location match (average 0) OK. Mesh OK. End I just needed a confirmation that my BC were reasonables. Just in case, here is a small movie of what's happening: http://www.box.com/s/8c79ad85af98d9405da9 Anyway I'm testing the case using a bigger domain... Daniele |
|
May 11, 2012, 04:35 |
|
#5 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 237
Rep Power: 16 |
Dear all, my cases with an outlet worked fine in OF 1.7.1 but now with OF 2.1.x there is no outflow anymore, alpha1 gets reflected at the outflow. Is there a change in the versions? otherwise it must be due to some changes i did in the fvSchemes and fvSolution files...
|
|
May 11, 2012, 06:04 |
|
#6 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 237
Rep Power: 16 |
using PISO instead of PIMPLE solves the problem
|
|
May 23, 2012, 06:27 |
|
#7 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 237
Rep Power: 16 |
Ok turning old searching the cause of alpha1 being reflected at the outflow, I finally got it (its not about PISO or 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 whol gid lies at a position that the x-coordinates are smaller than 0 the outflow works! Maybe this should be reported.
|
|
June 14, 2012, 09:00 |
|
#8 |
Senior Member
Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 237
Rep Power: 16 |
I changed p_rgh from type outletInlet outletValue uniform 0 to zeroGradient and the reflection of alpha1 at the outlet vanishes. Anyway I'd be happy for any explanation why a shift of the grid from negative to positive coordinate system quadrant can cause such behavior when outletValue uniform 0 is used for p_rgh.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
not outflow at outlet in interFoam | deniggo | OpenFOAM | 15 | May 17, 2022 06:06 |
Outlet boundary condition for wave flume with interFoam solver | Arnoldinho | OpenFOAM | 9 | July 10, 2018 05:15 |
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 |
Outlet boundary condition for pd in InterFoam | gopala | OpenFOAM Running, Solving & CFD | 0 | March 19, 2008 09:26 |