[maka]

y is initialized to GREAT as a result above the cutOff the expression reduces to:

min(geometricDelta_(), GREAT)

This is according to the following comment:

Description
Holds information (coordinate and yStar) regarding nearest wall point.
Used in VanDriest wall damping where the interest is in y+ but only
needs to be calculated upto e.g. y+ < 200. In all other cells/faces
(since y gets initialized to GREAT and yStar to 1) the damping function
becomes 1

Best regards,
Maka.

[philippebv]

Hi,

I'm running LES with the oodles solver and the Spalart-Allmaras formulation for the LESmodel. I would like to know which LES delta to use in order to have delta=max(deltaX,deltaY,deltaZ). I think it is more appropriate for DES calculation but correct me if I'm wrong.

Also, I'm using the backward scheme for time derivative and I went through some problems with convergence. The backward scheme is unconditionally stable but my calculation fails after a certain time. The cause is still unknown but I wonder if I could use a better scheme for the time derivative.

Thanks for your help,

Philippe

[philippebv]

Good morning,
I used a RANS solution to initialize my DES calculation and it solved the convergence problem.

Still, I would like to know how to set delta=max(deltaX,deltaY,deltaZ) instead of using cubeRootVol. It would be much appreciated if anyone could give me this quick information.

Regards,

Philippe

[eugene]

There is no way, short of implementing it yourself.

We never added this option for several reasons:
1. There is no unambiguous way to define deltaX,Y,Z on an unstructured mesh (or at least no easy way).
2. Tests on plane diffusers showed better behaviour using cuberoot of the volume. Admittedly these internal flow test cases were not ideal.
3. There is not that much difference in the value of delta except that the cuberoot method provides a smooth transition while the max method is discontinuous.

[kar]

Hello,
I hope this is an appropriate place to ask about LES computational requirements - I know, that it can be very problem-specific, but what would be your estimation for learning purposes? I mean, to gain enough knowledge, to be ready for some serious solving!

[philippebv]

Thank you Eugene,

I referred to your thesis (4.5 Errors and Mesh Refinement) and the smoothed delta indeed makes more sense. I will investigate the smooth option for the LES delta.

Best regards,

Philippe

[nikhilmadduri]

hello,
I was trying a LES for a turbulent flow over a circular cylinder. I have generated the mesh required but I am facing difficulty in running it for a particular set of parameters. Infact a simple cylinder case must be very easy but I dunno why I was ending up with all these following errors. I was implementing it for the case - rhoTurbFoam. Could anyone please help me out in running it successfully. And please also suggest what all parameters that I have to be ready with before running the simulation.


#0 Foam::error::printStack(Foam:stream&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hc onstthermo<foam::perfectgas> > > > >::calculate() in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysical Models.so"
#4 Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hc onstthermo<foam::perfectgas> > > > >::hThermo(Foam::fvMesh const&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysical Models.so"
#5 Foam::basicThermo::addfvMeshConstructorToTable<foa m::hthermo<foam::puremixture<f oam::consttransport<foam::speciethermo<foam::hcons tthermo<foam::perfectgas> > > > > >::New(Foam::fvMesh const&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysical Models.so"
#6 Foam::basicThermo::New(Foam::fvMesh const&) in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysical Models.so"
#7 main in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoTurbFo am"
#8 __libc_start_main in "/lib/i686/libc.so.6"
#9 Foam::regIOobject::readIfModified() in "/home/caelinux/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/rhoTurbFo am"

replies will be highly appreciated.
thanq
--Nikhil.

[lakeat]

> Could anyone please help me out in running it successfully. And please also suggest what all parameters that I have to be ready with before running the simulation.

rhoTurbFoam for LES?
hi Nikhil, I think it would be a good habit for you to post questions in a more detailed way, such as you set-up, case discreption, etc.

Regards,
Daniel

[lakeat]

A nice day to you all!
Could someone write a manual of LES? I am having a hard time with LESProperties now. That would be very nice for the new Foamer.

I have question concerning wall Function of LES in OpenFOAM.
1. Does LES in OpenFOAM use wall function? For I can't see any references of class nuSgswallFunctionFVpatchscalarField except in these two files, namely:
nuSgswallFunctionFVpatchscalarField.H
nuSgswallFunctionFVpatchscalarField.C

Regards, Daniel

[lakeat]

Another question concerning new models of LES,

The 1st one is You, D. and Moin, P. (2007), "A dynamic global-coefficient subgrid-scale eddy-viscosity model for large-eddy simulation in complex geometries", Physics of Fluids.

The other is WALES.

So, could any one shine some lights on how to implement them in OF. Is it possible? Is it easy?

Thanks a lot!
Daniel

[lakeat]

Dear developers:

On the development of LES in OpenFOAM, what are your main concerns now? New LES models or wall treatment, or whatelse?

What is the strength and weakness of LES in OF comparing with Fluent? Could you give me a little comments. Thank you.

I am sorry for so many questions.
Oh, this page is too long, why not divide it?

Best Regards, Daniel

[guanghaowu]

Hi, Wei

As far as I know, Foam does not use wall functions in the LES models. You may use smaller mesh size near the boundary or use dynamic LES models.

It is not so difficult to add a new LES model to OF. If you familiar with FOAM, you probably need 2-4 weeks(?) to do that.

You may refer to other existing dynamic LES models like dynSmagorinsky. Anyway, reading LESModel, LESdelta and LESfilter in detail is necessary to implement a new dynamic LES model.

[cedric_duprat]

Hi Daniel and Guanghao,

About wall model, there are lots of way to check if there is or not wall model in OF for LES:
1- shearch for "wall model LES" and you will find in this thread discussion between Eugene de Villier and Rolando Maier about this question.
2- have a look on the only LES pH'D thesis on OpenFOAM (Eugene de Villier's one) and you will find all the details and more.

"What is the strength and weakness of LES in OF comparing with Fluent?"
Quite easy, if you whant to implement your own SGS model in LES or your own wall model, it's easier

about LES SGS model, the main reference is Fureby C.et al. Phys. Fluids, Vol. 6, No. 11, 1997 "Differential subgrid stress models in LES"

hope it helps,

Cedric

[lakeat]

Thank you, 吴老师, your information is very helpful!

Regards, Daniel

[lakeat]

Hello Cedric, Thanks for sharing and help!
Much appreciated.

Daniel

[philippebv]

Hi Daniel,

I might add that a concern for LES is the calculation of delta. Indeed, nuSgs being related to the grid size, the method for the calculation of delta can have great influence. It becomes a big concern if you want to use a DES approach because delta triggers the transition between the RANS and the LES. In any way, you will also find information on this regard in Eugene de Villier's thesis.

Best,

Philippe

[lakeat]

Dear foamers,
I have difficulties in initialize the field?
My ultimate question is how to set k and nuSgs field?
What principles shall I respect and observe?

For my test case is flow past a square cylinder, the b.c. are
1) Symmetry conditions at the lateral boundaries
2) Free slip boundary conditions were used on the top and bottom domain boundaries.
3) Convective boundary conditions at the downstream boundary. With the help of Takuya.*
4) No-slip boundary conditions at the cylinder surface.
5) Inflow velocity is set to uniform so that Re=22000;
6) Outlet p is set as fixedValue zero.

It seems no big trouble for me to set U & p field, but what about the k & nuSgs?
I have read the UG, and see how in turbFoam's cavity case to set k field, but I still have no good idea.

I remember Eugene said

p=0 and small k is fine.
nuSgs doesn't matter because it is calculated from k and delta.

So, are the following setting okay?
<pre>*******************initial k*********************************start
internalField uniform 0;
boundaryField
{
cylinder
{
type fixedValue; //zeroGradient????
value uniform 0;
}
lateral1
{
type symmetryPlane;
}
lateral2
{
type symmetryPlane;
}
inlet
{
type fixedValue;
value uniform 2e-05; //zero or zeroGradient or a small value??
}
outlet
{
type inletOutlet; //zeroGradient or what..?? Why inletOutlet is preferred?
inletValue uniform 0; //If inletOutlet, then how to set these 2 value properly?
value uniform 0;
}
slip
{
type slip;
}
}

*******************initial k***********************************end

*******************initial nuSgs*****************************start
internalField uniform 0;
boundaryField
{
cylinder
{
type zeroGradient;
}
lateral1
{
type symmetryPlane;
}
lateral2
{
type symmetryPlane;
}
inlet
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}
slip
{
type slip;
}
}

*******************initial nuSgs*******************************end</pre>

Please advice, Thanks!

Daniel

[eugene]

Its generally not a good idea to set k to zero. Rather use something like 1e-10.

Unless your walls are well resolved, you should put nuSgsWallFunction on the nuSgs BCs for walls.

InletOutlet, is a zeroGradient boundary when the flow is outward and a fixed value boundary when the flow is coming in. The inlet value is the level in case of inflow.

[philippebv]

Hi foamers,

@ Eugene, what would be the correct yPlus values at walls when using nuSgsWallFunction?

Thanks,

Philippe

[eugene]

Somewhere between 0 and 300. Although if it is larger than about 10 you will be doing some kind of DES.