|
[Sponsors] |
November 23, 2012, 06:32 |
Inappropriate boundary conditions?
|
#1 |
New Member
Join Date: Sep 2012
Location: Germany
Posts: 25
Rep Power: 13 |
Hello everyone!
I want to ask, if you might take a look into my following case? The calculations abort after ten or some more iterations due to an excessively raising Courant number. Apparently the fast raising velocity U causes the solver to give up. In my experience most cases aborted in consequence of wrong boundary conditions, but I can't see any mistakes there. (see codes below) The model is a flow channel (see attachment 'model) which has an inlet 'einlass' on its upper side (green) and an outlet (red) below. The wall 'wand' is yellow. Postprocessing the few time steps before the calculations stop shows me results I really don't understand. Time step 1 (1.jpg) seems okay, but time step 11 (11.jpg) already shows an outrageous high velocity U. The BCs: U Code:
dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { einlass { type fixedValue; value uniform (1e-3 0 0); } auslass { type zeroGradient; } wand { type fixedValue; value uniform (0 0 0); } } Code:
dimensions [0 2 -2 0 0 0 0]; internalField uniform 1; boundaryField { einlass { type zeroGradient; } auslass { type fixedValue; value uniform 1; } wand { type zeroGradient; } } Code:
transportModel CrossPowerLaw; CrossPowerLawCoeffs { nu0 nu0 [ 0 2 -1 0 0 0 0 ] 300000; nuInf nuInf [ 0 2 -1 0 0 0 0 ] 50; m m [ 0 0 1 0 0 0 0 ] 2.5; n n [ 0 0 0 0 0 0 0 ] 0.8; } Salome meshes without errors and checkMesh is happy, too. (see below) Code:
Mesh stats points: 5378 faces: 46288 internal faces: 39840 cells: 21532 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 21532 polyhedra: 0 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 einlass 908 503 ok (non-closed singly connected) auslass 116 77 ok (non-closed singly connected) wand 5424 2778 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-0.15 -0.0559199 -0.125) (-0.0297394 0.045 -0.035) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (3.0834e-16 2.71627e-17 8.63031e-17) OK. Max cell openness = 2.25618e-16 OK. Max aspect ratio = 30.2779 OK. Minumum face area = 1.31017e-09. Maximum face area = 9.67659e-05. Face area magnitudes OK. Min volume = 2.37245e-13. Max volume = 3.29188e-07. Total volume = 0.000503545. Cell volumes OK. Mesh non-orthogonality Max: 84.4948 average: 19.033 *Number of severely non-orthogonal faces: 10. Non-orthogonality check OK. <<Writing 10 non-orthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 1.41613 OK. Coupled point location match (average 0) OK. Mesh OK. End Regards Sebastian |
|
November 23, 2012, 06:44 |
|
#2 |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 |
Can you use hex or polyhedral cells instead of tetrahedral? Tets are known to behave badly. If there is swirl at the exit, you might want to try inletOulet for velocity. Also, it has been noted in the forum and from my own personal experience, that fixedMeanValue for pressure can be a little more stable. However, I have only used that BC in steady-state problems. Lastly, how does a steady-state solver perform, can you get a SS solution?
|
|
November 23, 2012, 10:32 |
|
#3 |
New Member
Join Date: Sep 2012
Location: Germany
Posts: 25
Rep Power: 13 |
Thanks for your response, chegdan!
I use Salome for the meshing... What would you recommend? The BC inletOutlet unfortunately didn't solve my problem, but I have to admit, that I am not sure, if i used it correctly. I integrated it for the velocity U at the outlet. Would you use it for pressure BCs, too? Concerning the fixedMeanPressure I didn't try it until now. Did I read correctly, that I have to compile it from other sources? Sebastian |
|
November 23, 2012, 11:10 |
|
#4 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Have a look at http://www.cfd-online.com/Forums/ope...condition.html for a link (and some explanation) to the sources of the fixedMeanValue boundary condition.
Do you let your time step to be determined dynamically (i.e. based on the courant number)? If not, try to run the case with pimpleFoam (or the equivalent if its not an incompressible flow) and set the maximum courant number < 1. Greetz, L |
|
November 23, 2012, 11:21 |
|
#5 | |
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 |
Sebastian,
If you can get an stl out of salome for the surfaces, you might want to give snappyHexMesh a try and generate Hex cells. If you want to go the arbitrary polyhedral mesh route, you can generate a Delaunay triangulate tet mesh and then convert it to arbitrary polyhedral using polyDualMesh. fixedMeanValue is in the extend version of OpenFOAM and you can get the code and compile it with minimal effort. There is a discussion located at http://www.cfd-online.com/Forums/ope...condition.html. Good luck and have a great weekend! Quote:
|
||
January 17, 2013, 08:08 |
|
#6 | |
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Beijing, China
Posts: 838
Rep Power: 17 |
Quote:
|
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Impinging Jet Boundary Conditions | Anindya | Main CFD Forum | 25 | February 27, 2016 12:58 |
symmetry boundary conditions in cfx | lost.identity | CFX | 41 | May 22, 2013 07:21 |
OpenFOAM Variable Velocity Boundary Conditions | NickolasPl | OpenFOAM Programming & Development | 2 | May 19, 2011 05:37 |
[Netgen] boundary conditions and mesh exporting | vaina74 | OpenFOAM Meshing & Mesh Conversion | 2 | May 27, 2010 09:38 |
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues | michele | OpenFOAM Meshing & Mesh Conversion | 2 | July 15, 2005 04:15 |