[7islands]

We are in the process of validating OpenFOAM against other CFD codes, wind tunnel tests and field measurements using benchmarking test cases defined by a Japanese academic society (or its journal article if you prefer paper form) for urban wind environment predictions. If you follow the link you'll find 8 cases, cases A - H, simulating urban environments with varying reality, ranging from simple blocks to realistic urban terrains. Among those we have finished cases A - F, and in the process of publishing the case data so that any OpenFOAM users can reproduce our results. The test cases Elvis mentioned

Originally Posted by elvis

http://openfoamwiki.net/index.php/Ma...banAreaNiigata
http://openfoamwiki.net/index.php/Ma...ngInCityBlocks

are cases E and D respectively which my colleague (the author of the aforementioned presentation slides) has just published. We should be able to publish other cases as well shortly, among them cases E and F are realistic sHM cases enough to get an idea about how sHM works for urban terrains.

Takuya

[imano]

Hi Guillaume,

I'm sorry for late reply.

I'd like to answer your 1st and 4th questions (thanks a lot Takuya for
answering 2nd and 3rd)

Originally Posted by Voyage_gui

- from a clean CAD file (after post-processing of aerial laser scanned geographical data), how long did it take him to mesh the whole district ?

It takes about one hour in 16 cpu parallel as listed below:

blockMesh (in single): 1 min.
decomposePar (in single): 1 min.
snappyHexMesh (in 16 cpu parallel): 40 mins.
reconstructParMesh (in single): 17 mins.

Originally Posted by Voyage_gui

- Does he have any papers regarding urban design ?

My English papers for CFD prediction of urban environment are very few so
far, but have a look at e.g.:

http://dl.dropbox.com/u/3609076/Vent...per_ver.2_.pdf
http://dl.dropbox.com/u/3609076/Vent...2009100201.pdf

Originally Posted by Voyage_gui

7islands : Thks for the LES presentation. Too bad i don't know japanese (by any chance same document in English?). Was he satisfied by the result of the DES simulation (any exp. measure to compare with) ?
Guillaume

There is no English document for this presentation, sorry.
Moreover I couldn't validate LES or DES simulation since I didn't have
any measurement data to compare with in this case.

As Elvis and Takuya mentioned in previous posts, I uploaded
OpenFOAM tutorial cases which predict urban wind environment and
validate with wind tunnel measurement data.
Though these cases use RAS model as turbulent model, but it's easy to
change it to VLES or DES if you share the mesh for the RAS calculation.
So please try validating these benchmark tests with VLES or DES model
and report the results if you have spare time

Masashi

[izna]

hello..

I am hijacking this post.
I am simulating a flow over an urban area, but i am working in 2D, i am obtaining convegence with simpleFOam but when view in paraview its as if no wind has enter my domain..

Can you please advice me on the boundary conditions used? I tried SLip and inletoutlet all in vain...

I am using RAS model, with GAMG solver .

My east side of domain is inlet and the three remaining sides ie north south and west are outflow where my wind is supposed to go ...
But i need help in the boundarycondition..

kind regards
izna

[julien.decharentenay]

Izna,

Probably best to create a new post for your question...

Can you post your U and p directory?

Julien

[izna]

hi.. thanks a lot for the reply.. below is my u and p dire.. also sides means the north and south sides... its in 2D

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
wall
{
type fixedValue;
value uniform (0 0 0);
}
outflow
{
type zeroGradient;

}

inlet
{
type fixedValue;
value uniform (-4 0 0);
}
sides
{
type fixedValue;
value uniform (0 0 0);
}

frontAndBackPlanes
{
type empty;
nFaces 67650;
startFace 68115;
}
}

// ************************************************** *********************** //

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
wall
{
type zeroGradient;
}
outflow
{
type fixedValue;
value uniform 0;
}

inlet
{
type zeroGradient;
}

sides
{
type zeroGradient;
}
frontAndBackPlanes
{
type empty;
nFaces 67650;
startFace 68115;
}
}

// ************************************************** *********************** //

[julien.decharentenay]

Thanks. Nothing obviously wrong with the two files. Can you send some more information (mesh, solver output, screenshot)?

[izna]

hi.. meshwas done in Gambit.. converted to FOam..
solver PCG i am putingh FV solution here

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0.1;
}

pFinal
{
solver PCG;
preconditioner DIC;
tolerance 1e-06;
relTol 0;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

k
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

epsilon
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

R
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

nuTilda
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}
}

SIMPLE
{
nNonOrthogonalCorrectors 0;

residualControl
{
p 1e-2;
U 1e-3;
"(k|epsilon|omega)" 1e-3;
}
}
residualControl
{
p 1e-3;
U 1e-4;
"(k|epsilon|omega)" 1e-3;
}


// ************************************************** *********************** //

each time after certain number of iterations i obtain my program is crashing..hence one picture which i was able to view before crashing.. you can clearly see that in thsi pic, thhe simulations was partly stopped...

[izna]

we can see it has not simulated to convergence.. but how to make it converge without crashing???

[izna]

when i do the BC as symmetryPlane i obtain the errors...

Create time


Create mesh for time = 0


Reading field p


Reading field U


Reading/calculating face flux field phi


Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
--> FOAM Warning :
From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/Field.C at line 262
Reading "/home/izna/Desktop/y/0/k" from line 18 to line 54
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}


No finite volume options present




SIMPLE: convergence criteria
field p tolerance 0.01
field U tolerance 0.001
field "(k|epsilon|omega)" tolerance 0.001




Starting time loop


Time = 1


DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 3.07582883344e-05, No Iterations 1001
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.95605000958e-06, No Iterations 301
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.0999726835198, No Iterations 584
time step continuity errors : sum local = 29.8522772566, global = -0.0024880751966, cumulative = -0.0024880751966
DILUPBiCG: Solving for epsilon, Initial residual = 0.999913801056, Final residual = 1.00016301843, No Iterations 1001
bounding epsilon, min: -219.225697355 max: 207.638755413 average: 0.998265362431
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 1.13408135894e+12, No Iterations 1001
bounding k, min: -4.17424118765e+16 max: 8.29450514701e+16 average: -1.52614847385e+12
ExecutionTime = 424.6 s ClockTime = 425 s


Time = 2


DILUPBiCG: Solving for Ux, Initial residual = 0.801813491704, Final residual = 0.801813491704, No Iterations 1001
DILUPBiCG: Solving for Uy, Initial residual = 0.659490592026, Final residual = 0.659490592026, No Iterations 1001
DICPCG: Solving for p, Initial residual = 0.999998931991, Final residual = 2762872.03121, No Iterations 1001
time step continuity errors : sum local = 7.05385314245e+12, global = 12013.6485228, cumulative = 12013.6460347
DILUPBiCG: Solving for epsilon, Initial residual = 0.246233904231, Final residual = 369.290447986, No Iterations 1001
bounding epsilon, min: -1.8042009224e+36 max: 6.34190622628e+35 average: 2.79678186829e+31
DILUPBiCG: Solving for k, Initial residual = 1.62772660345e-13, Final residual = 1.62772660345e-13, No Iterations 0
ExecutionTime = 814.39 s ClockTime = 816 s


Time = 3


#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam:ILUPreconditioner::calcReciprocalD(Foam::Fi eld<double>&, Foam::lduMatrix const&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#4 Foam:ILUPreconditioner:ILUPreconditioner(Foam: :lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix:reconditioner::addasymMatrixCons tructorToTable<Foam:ILUPreconditioner>::New(Foam ::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix:reconditioner::New(Foam::lduMatr ix::solver const&, Foam::dictionary const&) in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam221/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#8
in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/simpleFoam"
#9
in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/simpleFoam"
#10
in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/simpleFoam"
#11
in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/simpleFoam"
#12 __libc_start_main in "/lib/i386-linux-gnu/libc.so.6"
#13
in "/opt/openfoam221/platforms/linuxGccDPOpt/bin/simpleFoam"
Floating point exception (core dumped)

[julien.decharentenay]

Izna,

What is your question/request for assistance?

Your post 9.10:

i am obtaining convegence with simpleFOam but when view in paraview its as if no wind has enter my domain

Your post 10.10:

we can see it has not simulated to convergence.. but how to make it converge without crashing???

[izna]

i am sorry.. its just i am trying a lot of different solvers..

My question is i want to obtain a velocity start from the east side of my domain.. but i am obtaining the followig picture..

[julien.decharentenay]

No drama. It is getting clearer. I can't see anything wrong from the dictionary, but have to admit that I have not done 2D simulations... So there are a few of the "tricks" that I do not know.

Could you post a link to a complete case for download and try?

[izna]

yesh am going to send a link..thnaks heaps Julien..

[julien.decharentenay]

Hi Izna,

Thanks for sending the case through. It helps - even though I have not tried to run the model. Below are two suggestions:

1) North and South boundaries:

In your setup, these are defined as "outlet" boundary conditions. I understand that you are using this approach as you would like to allow for exit/re-entry of fluid. This set of condition is what creates in your case the high in-velocity observed in the picture.

My recommendation is to change these conditions to symmetry (for the north and south faces only). If you are concerned about flow exit/re-entry, you can evaluate the impact of the domain size (in width) on the variable of interest by doubling the domain size in the width direction.

2) West boundary condition:

The setup is a zero velocity gradient and zero pressure. I personally prefer to change it to an inlet/outlet setup where the backflow velocity is specified as zero. It operates as the outlet you defined as long as the flow is going out, but prevent backflow. I found this approach more stable. Although this may have some impact, the above suggestion should be sufficient.

Let me know if you try any of the above and if they work (as a separate thread).

[izna]

hello Julien
http://www.cfd-online.com/Forums/ope...tml#post456673


this is the new thread please do check.



izna

[Mark JIN]

Hey Guys, your discussions are really helpful, thanks!