# Urban scenario - tetra vs hex problem

 Register Blogs Members List Search Today's Posts Mark Forums Read

 March 30, 2009, 13:05 Urban scenario - tetra vs hex problem #1 New Member   Pablo Grazziotin Join Date: Mar 2009 Posts: 6 Rep Power: 9 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 non-orthogonality Max: 65.5343 average: 19.5644 Non-orthogonality 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 non-orthogonality? Or is my problem something else entirely? Thanks, -Pablo

 March 30, 2009, 13:20 #2 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 9 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 fine-mesh 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: 12
Quote:
 Originally Posted by pablocg Is there some simple way of determining the number of correctors based on the mesh non-orthogonality?
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: 9 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 3-4 steps. Any other ideas? Thanks.

 April 2, 2009, 03:46 #5 Senior Member   matej forman Join Date: Mar 2009 Location: Brno, Czech Republic Posts: 104 Rep Power: 9 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: 9
Quote:
 Originally Posted by matejfor Hi, Just to make sure, do you have some prism layer in your tet mesh?
I'm not sure, think not... Am using GAMBIT size functions and Tet/Hybrid elements. To be honest, I hadn't heard of such issue before...

Quote:
 Originally Posted by matejfor What BC you have for epsilon and k at inlet? Are they realistic? and initial condition?
These are fine. U, k and epsilon are based on the following equations:

Uinlet == ufric*log((z+z0)/(Ka*z0)) * vector(1,0,0);
kinlet == ufric2/::sqrt(0.09);
epsiloninlet == ufric2*ufric/(Ka * (z+z0));

Quote:
 Originally Posted by matejfor 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.
No, havent tried this yet.

Quote:
 Originally Posted by matejfor How does your fvSchemes look like? matej
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 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;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(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;
}

{
default corrected;
}

fluxRequired
{
default no;
p;
}

Any help/ideas/suggestions are appreciated.
Thanks,
-Pablo

 April 9, 2009, 03:14 #7 Senior Member   matej forman Join Date: Mar 2009 Location: Brno, Czech Republic Posts: 104 Rep Power: 9 Hi, by prism layer I mean a layer of typically prism-shaped 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 Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ParodDav CFX 5 April 29, 2007 19:13 Baskaran CFX 2 March 13, 2006 13:59 Forrest CFX 4 May 25, 2005 18:37 Mikhail Main CFD Forum 40 September 9, 1999 09:11 Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52

All times are GMT -4. The time now is 09:38.