# Wind on building simulation

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

August 25, 2014, 11:00
Wind on building simulation
#1
New Member

Cedric
Join Date: Jun 2014
Location: France
Posts: 16
Rep Power: 11
Hi everybody,
I 'm trying to perform a simulation of wind on a building in order to know the pressure on a particular part of a building roof.
I follow the simplefoam/motorbike tutorial and I adjust it to my case. But when I try to see the result in paraview, it's wrong!(pictures).
I think it can be a problem of dimensions in my blockMesh but I tried different solutions and I failed.
Could somebody explain me why it doesn't work please ? (I'm a beginner in OF)
Attached Images
 essai2_st_2.jpg (9.5 KB, 180 views) essai2_st_3.jpg (11.9 KB, 134 views) essai2_st_1.jpg (9.3 KB, 106 views)

 August 25, 2014, 21:29 #2 Member   Gregoire Junqua Join Date: Jun 2011 Location: China Posts: 58 Blog Entries: 1 Rep Power: 14 what is your inlet condition? (by the way the others) Don't forget that you are in ABL condition many things need to be change. And then motorbike simulation don't agree with your simulation what is your domain size compare to the building size?

August 26, 2014, 05:18
#3
New Member

Cedric
Join Date: Jun 2014
Location: France
Posts: 16
Rep Power: 11
Hi,
I'm a very beginner and I guessed I just had to "replace" the motorbike by my own geometry. I'm not sure to understand what you mean by Inlet Condition but I attached some files I hope it's what you mean.

I'am doing research on ABL as you advised to me but, for the moment, I have not the solution.

You said the motorbike tutorial wasn't the good one, could you advise me an other one?

About my domain size : If I call L the maximum lenght of my building, il have 3L between my building and the inlet, 3L on each side and 8L behind.

Attached Files
 fixedInlet.txt (700 Bytes, 53 views) frontBackUpperPatches.txt (704 Bytes, 23 views) initialConditions.txt (778 Bytes, 42 views)

 August 27, 2014, 20:20 #4 Member   Gregoire Junqua Join Date: Jun 2011 Location: China Posts: 58 Blog Entries: 1 Rep Power: 14 My meaning is that you are in atmospheric boundary layer condition. So you need to apply a log-law (or the power law) on the inlet and change the inlet accordingly to the epsilon (or omega) and to the Turbulent Kinetic Energy (TKE can stay in fixed value). You can have a try with the boundary condition in the turbineSitting tutorial located in the simpleFoam's tutorial part. There you will have the different inlet (k-epsilon) and also you can use the nut bottom boundary to model grass or road around your buildings. regards GJ

 September 4, 2014, 10:40 #5 New Member   Cedric Join Date: Jun 2014 Location: France Posts: 16 Rep Power: 11 Hello GJ, Unfortunatly, I have no time to work on it until today. I look at the tutorial you advice me and I think I understand what mean ABLC now but I steel don't see how to change my inlet to have a log-law. Indeed, I undersatnd why I must do it but as I am a very beginner in C++, I can't see how to set up it in an OpenFoam file... Thank you very much for your help, Regards Cedric

 September 4, 2014, 23:25 #6 Member   Gregoire Junqua Join Date: Jun 2011 Location: China Posts: 58 Blog Entries: 1 Rep Power: 14 Hi there you needn't to program just look at tutorials/incompressible/simpleFoam/turbineSiting it show the different inlet for ABL layer epsilon : atmBoundaryLayerInletEpsilon k : uniformFixedValue nut : nutkAtmRoughWallFunction U : atmBoundaryLayerInletVelocity these are a little outdated inlet I suggest you to have a look of this article for parametrize your inlet Yang, Y., M. Gu, S. Chen, and X. Jin, 2009: New inflow boundary conditions for modelling the neutral equilibrium atmospheric boundary layer in computational wind engineering. Journal of wind engineering and industrial aerodynamic, 95, 88–95. f And you should lower the constant C_\mu of the bradshaw relationship from 0.09 to 0.03 And change the turbulent kinetic energy inlet accordingly namsivag likes this.

September 8, 2014, 12:45
#7
New Member

Cedric
Join Date: Jun 2014
Location: France
Posts: 16
Rep Power: 11
Hi,
I'm traying to adjust the turbinesiting tutorial to my case but there still is a file I don't understand everythings.
When I look at the Allrun, I undersand until SnappyHexMesh, after I cut off the topoSet "step" as I think it is useless (I also cut off fvOption). But I can't manage to run my case.
Here is the error message :
Quote:
 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 bounding k, min: 0 max: 1.3 average: 1.30000000001 bounding epsilon, min: 0 max: 0.577954048984 average: 0.0100000000001 kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; sigmaEps 1.11; } No finite volume options present SIMPLE: convergence criteria field p tolerance 0.001 field U tolerance 0.0001 field "(k|epsilon)" tolerance 0.0001 Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0850202022064, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0421649962824, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0820188872721, No Iterations 2 -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 31 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them. -------------------------------------------------------------------------- [0] [0] [0] --> FOAM FATAL ERROR: [0] No coarse levels created, either matrix too small for GAMG or nCellsInCoarsestLevel too large. Either choose another solver of reduce nCellsInCoarsestLevel. [0] [0] From function GAMGSolver::GAMGSolver(const word& fieldName,const lduMatrix& matrix,const FieldField& interfaceBouCoeffs,const FieldField& interfaceIntCoeffs,const lduInterfaceFieldPtrsList& interfaces,const dictionary& solverControls) [0] in file matrices/lduMatrix/solvers/GAMG/GAMGSolver.C at line 121. [0] FOAM parallel run exiting
Do you understand where the error could be?

September 10, 2014, 04:16
atmBoundaryLayerInletVelocity
#8
New Member

Cedric
Join Date: Jun 2014
Location: France
Posts: 16
Rep Power: 11
Hi, I worked on it the all day and I finally managed to have results for my own stl.
After that, I searched for renseignement on "U : atmBoundaryLayerInletVelocity" and there are somethings I can't anderstand and I hope you could help me.

As you can see in the pictures I attached, the results are diferents when I use Excel with the U atmBoundaryLayerInletVelocity equation and when I watch the same thing with Paraview.

Moreover I can't understand why there is no correspondance between the Href/Uref theoric (I put in the ABLConditions file in OpenFoam) and the Href/Uref I visualise paraview.

I hope I clear enought.
Regards,
Cedric
Attached Images
 20blabla.jpg (83.5 KB, 90 views) 100blabla.jpg (85.4 KB, 60 views) 200blabla.jpg (85.9 KB, 54 views) paramètres_ABL.jpg (89.9 KB, 66 views)

 September 10, 2014, 05:27 #9 Senior Member   Elvis Join Date: Mar 2009 Location: Sindelfingen, Germany Posts: 618 Blog Entries: 6 Rep Power: 23

 September 10, 2014, 10:13 #10 New Member   Cedric Join Date: Jun 2014 Location: France Posts: 16 Rep Power: 11 Hi Elvis, Thanks for your reply. I look at the 2 examples you adviced me. I guess it can be usefull to compare with my model when it will work but I still can't understand why I get this diffences between the theory (with excel) and the simulation (in OpenFoam) as I assume it the same equation at the base.

 September 15, 2014, 05:21 symmetrtPlane #11 New Member   Cedric Join Date: Jun 2014 Location: France Posts: 16 Rep Power: 11 Hi everybody, Now, I manage to perform a case with my building thank to your help. I have just an other question concerning the boundaries : why the tutorial "turbinesitting" doesn't use the condition "symmetrtPlane" on the sides and the top boundaries? Thanks for your replies, Regards, Cedric

 September 17, 2014, 11:58 #12 New Member   Cedric Join Date: Jun 2014 Location: France Posts: 16 Rep Power: 11 Hi, I had no understand what "symettryPlane" condition mean in OpenFoam, I use an other soft where it means that the conditions one the one side of the boundary is the same that on the other side, whereas in OF it means just a "basic" symmetryPlane which make a symetrie. It is usefull if you have a symetry on your domain for exemple but it's no use to define a boundary limit.

 September 17, 2014, 21:33 #13 Member   Gregoire Junqua Join Date: Jun 2011 Location: China Posts: 58 Blog Entries: 1 Rep Power: 14 if you use symettryPlane you need to link it to one other face. But it's only good for geometrical design (in order to save memory and time). slip condition is a good condition. you should have a look on the thesis : Wind resource in complex terrain with OpenFoam June 2011 by Benjamin Martinez (it s almost the same as turbine sitting tutorial) It's a very good thesis, everything is well explained from the boundary to the resolution. It helped me a lot. __________________ ------------------------------------------------------- Gregoire Junqua Ocean University of China PhD Oceanography/ABL turbulence -------------------------------------------------------

September 18, 2014, 05:26
#14
New Member

Cedric
Join Date: Jun 2014
Location: France
Posts: 16
Rep Power: 11
Hi Greg,
I'm trying to reproduce a study somebody else has done on an hospital, I manage to reproduce the general comportement but there are détails I still can't reproduce (picture).
In your opinion, where does the problem come from? The precision of the snappyHexMesh (I tried to incress it several times but I still can't have the comportement I joined my file) or an other parameter I don't see yet?
Attached Images
 recitculation.jpg (92.3 KB, 118 views)
Attached Files
 snappyHexMeshDict.txt (7.9 KB, 39 views)

 December 17, 2014, 05:21 hi! cedrik #15 New Member   fangyingwang Join Date: Dec 2014 Posts: 2 Rep Power: 0 hi!!cedrik! i can't found the these above advised by gregjunqua! could you sent it to me use email ? thanks

 Tags building, motorbike tutorial