CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

LES

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

Like Tree27Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 4, 2008, 09:08
Default y is initialized to GREAT as a
  #121
Senior Member
 
Maka Mohu
Join Date: Mar 2009
Posts: 305
Rep Power: 9
maka is on a distinguished road
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.
maka is offline   Reply With Quote

Old   July 4, 2008, 09:13
Default Hi, I'm running LES with th
  #122
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
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 is offline   Reply With Quote

Old   July 7, 2008, 09:49
Default Good morning, I used a RANS s
  #123
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
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
philippebv is offline   Reply With Quote

Old   July 7, 2008, 09:57
Default There is no way, short of impl
  #124
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   July 7, 2008, 10:47
Default Hello, I hope this is an appr
  #125
kar
Senior Member
 
Kārlis Repsons
Join Date: Mar 2009
Location: Latvia
Posts: 111
Rep Power: 8
kar is on a distinguished road
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!
kar is offline   Reply With Quote

Old   July 7, 2008, 11:38
Default Thank you Eugene, I referre
  #126
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
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
philippebv is offline   Reply With Quote

Old   July 13, 2008, 04:37
Default hello, I was trying a LES for
  #127
New Member
 
nikhil babu madduri
Join Date: Mar 2009
Posts: 17
Rep Power: 8
nikhilmadduri is on a distinguished road
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.
nikhilmadduri is offline   Reply With Quote

Old   July 28, 2008, 10:08
Default > Could anyone please help me
  #128
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to 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
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 3, 2008, 23:31
Default A nice day to you all! Could
  #129
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to 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
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 3, 2008, 23:38
Default Another question concerning ne
  #130
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to 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
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 3, 2008, 23:49
Default Dear developers: On the dev
  #131
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to 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
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 4, 2008, 02:04
Default Hi, Wei As far as I know, F
  #132
New Member
 
Guanghao Wu
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 15
Rep Power: 8
guanghaowu is on a distinguished road
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.
guanghaowu is offline   Reply With Quote

Old   September 4, 2008, 03:00
Default Hi Daniel and Guanghao, Abo
  #133
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   September 4, 2008, 03:30
Default Thank you, 吴老师, your inf
  #134
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Thank you, 吴老师, your information is very helpful!

Regards, Daniel
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 4, 2008, 03:37
Default Hello Cedric, Thanks for shari
  #135
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Hello Cedric, Thanks for sharing and help!
Much appreciated.

Daniel
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 4, 2008, 08:52
Default Hi Daniel, I might add that
  #136
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
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
philippebv is offline   Reply With Quote

Old   September 5, 2008, 22:36
Default Dear foamers, I have difficul
  #137
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to 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
Quote:
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
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   September 8, 2008, 08:16
Default Its generally not a good idea
  #138
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
solefire and songwukong like this.
eugene is offline   Reply With Quote

Old   September 9, 2008, 13:45
Default Hi foamers, @ Eugene, what
  #139
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
Hi foamers,

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

Thanks,

Philippe
philippebv is offline   Reply With Quote

Old   September 9, 2008, 16:23
Default Somewhere between 0 and 300. A
  #140
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Somewhere between 0 and 300. Although if it is larger than about 10 you will be doing some kind of DES.
eugene is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 03:27.