
[Sponsors] 
March 30, 2009, 13:05 
Urban scenario  tetra vs hex problem

#1 
New Member
Pablo Grazziotin
Join Date: Mar 2009
Posts: 6
Rep Power: 8 
Hello all!
I've been trying to run some cases of airflow around buildings using simpleFoam. Simulations seem to converge fine when using a hexahedral mesh. However, if I try the same case but with a tetrahedral mesh, I get fast increasing time step continuity and bounding epsilon errors. Any suggestions? Right now I'm trying increasing numbers of Non Orthogonal Correctors, but without much success. My checkMesh results showed Mesh nonorthogonality Max: 65.5343 average: 19.5644 Nonorthogonality check OK. Should I be using such correctors for this? And how many? Is there some simple way of determining the number of correctors based on the mesh nonorthogonality? Or is my problem something else entirely? Thanks, Pablo 

March 30, 2009, 13:20 

#2 
Senior Member

Hi Pablo,
I have some experience with coarse mesh on uniform flow around a cylinder. Here I use very coarse mesh(because I want to use the converged results as initial condition for my finemesh test case). After the residual for p and U is of order 10^(6), I see increasing time step continuity and bounding epsilon errors afterwards. But when I use fine mesh I have no such phenomena. Therefore, may I suggest to use fine mesh? Of course there maybe other reasons. Other friends could give you good suggestions Bin 

March 30, 2009, 14:01 

#3 
Senior Member
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11 
Let me highlight this question. Although I have no answer to this question it can be of highly practical interest for all of us using tetrahedral mesh!
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!" 

April 1, 2009, 09:41 

#4 
New Member
Pablo Grazziotin
Join Date: Mar 2009
Posts: 6
Rep Power: 8 
Still haven't managed to get this to run properly with tetrahedral.
I did refine the mesh around the building (testing with just 1 at the moment), but my time step continuity error goes to E+30 within 34 steps. Any other ideas? Thanks. 

April 2, 2009, 03:46 

#5 
Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 91
Rep Power: 8 
Hi,
Just to make sure, do you have some prism layer in your tet mesh? What BC you have for epsilon and k at inlet? Are they realistic? and initial condition? You may try mapFields from the hex mesh to tet and see if it is able to continue from a good solution field with tetmesh. How does your fvSchemes look like? matej 

April 6, 2009, 10:39 

#6  
New Member
Pablo Grazziotin
Join Date: Mar 2009
Posts: 6
Rep Power: 8 
Quote:
Quote:
Uinlet == ufric*log((z+z0)/(Ka*z0)) * vector(1,0,0); kinlet == ufric2/::sqrt(0.09); epsiloninlet == ufric2*ufric/(Ka * (z+z0)); Quote:
I'm using pretty much the simplest schemes for now, until I can get it to run properly so I can try to refine it: ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } Any help/ideas/suggestions are appreciated. Thanks, Pablo 

April 9, 2009, 03:14 

#7 
Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 91
Rep Power: 8 
Hi,
by prism layer I mean a layer of typically prismshaped elements in the boundary region for the BL better description. But your problem is not a quality of the solution but the existence of it. What you may try is some limiting off the convection terms, something like: div(phi,U) Gauss UpwindV cellLimited leastSquares 1.0; or maybe 0.5. My problem with divergence of epsilon and continuity is typically wrong BC setting, mainly of k and epsilon at inlet. I recall someone here recently suggesting setting epsilon for the initial condition 10 times higher then that of the inlet. good luck matej 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Adiabatic and Rotating wall (Convection problem)  ParodDav  CFX  5  April 29, 2007 19:13 
ICEM CFD 5.1 problem with tetra count  Baskaran  CFX  2  March 13, 2006 13:59 
ICEM meshing problem  Forrest  CFX  4  May 25, 2005 18:37 
extremely simple problem... can you solve it properly?  Mikhail  Main CFD Forum  40  September 9, 1999 09:11 
Is this problem well posed?  Thomas P. Abraham  Main CFD Forum  5  September 8, 1999 14:52 