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

problems with a DES (k-epsilon model) implementation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 7, 2009, 04:12
Default problems with a DES (k-epsilon model) implementation
  #1
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
Hi everyone,

at the moment I will try to implementation the k-eps model in a DES .

The base of code are the DES SpalartA, white the two new components k and epsilon.

my epsilon (Ldes) is defined as :

if (mesh_.changing())
{
epsilon_ =
pow(k_,(3/2))/min(CDES_*delta(),pow(k_,3/2))/epsilon_);
}

as next I add the two equations

tmp<fvScalarMatrix> epsEqn
(
fvm::ddt(epsilon_)
+ fvm::div(phi_, epsilon_)
- fvm::Sp(fvc::div(phi_), epsilon_)
- fvm::laplacian(DepsilonEff(), epsilon_)
==
C1_*G*epsilon_/k_
- fvm::Sp(C2_*epsilon_/k_, epsilon_)
);


and

tmp<fvScalarMatrix> kEqn
(
fvm::ddt(k_)
+ fvm::div(phi_, k_)
- fvm::Sp(fvc::div(phi_), k_)
- fvm::laplacian(DkEff(), k_)
==
G
- fvm::Sp(epsilon_/k_, k_)
);

Now the problem with the case, after a successful wmake libso compilation,
its not possible to run the code.

After the start with oodles, its occurs this error messages

Courant Number mean: 0 max: 0.00126355
#0 Foam::error:rintStack(Foam::Ostream&) in "/usrfem/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/usrfem/femsys_local/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/usrfem/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usrfem/femsys_local/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/usrfem/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#6 Foam::incompressible::LESModels::kEpsilon::correct (Foam::tmp<Foam::GeometricField<Foam::Tensor<doubl e>, Foam::fvPatchField, Foam::volMesh> > const&) in "/usrfem/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#7 Foam::incompressible::LESModel::correct() in "/usrfem/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#8 main in "/usrfem/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/oodles"
#9 __libc_start_main in "/lib64/libc.so.6"
#10 Foam::regIOobject::readIfModified() in "/usrfem/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/oodles"
Floating exception


I hope I get some tips with this message or any helps how they test the turbulence model of errors



best regards
Sven









sven82 is offline   Reply With Quote

Old   April 8, 2009, 03:13
Default
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
without knowing anything about your model:

http://openfoamwiki.net/index.php/HowTo_debugging
mattijs is offline   Reply With Quote

Old   April 14, 2009, 07:53
Thumbs up
  #3
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
hi mattijs,

thanks for the link,
now its works fine

sven
sven82 is offline   Reply With Quote

Old   April 14, 2009, 08:41
Default
  #4
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
Hi, sven!

I'm very interested in your implementation, what's going on and which testCase do you use?

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   April 14, 2009, 10:08
Default
  #5
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
Hi Daniel,

before I start with some test case, I will try to implantation a flux blending between CDF and upwind.

In my opinion is the best test case cube with 3 cyclic patches in three mesh sizes with the target to compare the isotropic turbulence.
After this I will try a practice case like mirror of a car, something like this.

But the next step is the flux blending...........

Sven
sven82 is offline   Reply With Quote

Old   April 18, 2009, 06:00
Default
  #6
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Sven,

did you take a look at localBlended scheme? It should be suitable for this case.

Fabian
braennstroem is offline   Reply With Quote

Old   April 21, 2009, 10:31
Default
  #7
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
Hi braennstroem ,

the idea with the localblended sounds good and its definitely the simplest way for me,
thanks for that!

Sven
sven82 is offline   Reply With Quote

Old   April 30, 2009, 07:32
Default
  #8
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
Hi Sven,

How's it going?
I saw you have added the new L_DES scale, what is your reference papers, can you email me a copy of them? EMail: LAKEAT AT GMAIL DOT COM

Quote:
Originally Posted by sven82 View Post
before I start with some test case, I will try to implantation a flux blending between CDF and upwind.
As I remember, it seems they (the Desider community) used to use different schemes in RANS region and LES region, is this what you are trying to do?

Thank you!
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   May 4, 2009, 11:04
Default
  #9
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
hi lakeat,

thats exactly what I try do.

based of a empirical function like this



will I switch or mix the both schemes (upwind / central) !

(sorry for the bad picture ! klick to enlarge)

[TARVIN SHUR STRELETS SPALART (2002) Upgrades in the DES of complex turb. flow]
www.springerlink.com/index/m516557444083t38.pdf

when everything got a god idea for the implementation of the procedure or a similary example please post that here.

thx
Sven
sven82 is offline   Reply With Quote

Old   May 4, 2009, 11:09
Default
  #10
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
Hi braennstroem ,

the idea with the localblended sounds good and its definitely the simplest way for me,
thanks for that!

Sven
sven82 is offline   Reply With Quote

Old   May 4, 2009, 11:13
Default
  #11
Member
 
Sven Degner
Join Date: Mar 2009
Location: Zürich
Posts: 54
Rep Power: 8
sven82 is on a distinguished road
hi lakeat,

thats exactly what I try do.

based of a empirical function like this



will I switch or mix the both schemes (upwind / central) !

(sorry for the bad picture ! klick to enlarge)

[TARVIN SHUR STRELETS SPALART (2002) Upgrades in the DES of complex turb. flow]
www.springerlink.com/index/m516557444083t38.pdf

when everything got a god idea for the implementation of the procedure or a similary example please post that here.

thx
Sven
sven82 is offline   Reply With Quote

Old   May 5, 2009, 07:56
Default
  #12
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
I cannot download it, it's not free for my university. Can you email me a copy, thanks a bunch.
And did you notice the S-A model differences between
  1. http://www.cfd-online.com/Wiki/Spalart-Allmaras_model
  2. Wilcox-Turbulence Modeling for CFD
  3. Implementation in OpenFOAM
  4. Original S-A, in 1994
  5. Version published by Niktin
I am using Niktin's version, but I'm Just curious, How did OpenFOAM's version come?

Have you tried IDDES, it seems the length scale has changed a lot.

About the mixture of two schemes, is it stable and is it very NECESSARY for the simulation? I doubt that. Any ideas?
__________________
~
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   May 15, 2009, 12:42
Default
  #13
Member
 
Philippe B. Vincent
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 32
Rep Power: 8
philippebv is on a distinguished road
Hi Daniel, Sven, Fabian and other DES players,

Your work on DES implementation is very interesting. I was wondering if any of you tried to implement a DES-SST model? The proposed model by Strelets et al (AIAA Paper 2001-0879) is interesting. There is also a "shielded" formulation for that model, similar the DDES implementation in the Spalart-Allamaras model. That latter DDES-SA model can easily be implemented from the DES-SA already available in OpenFOAM (Ask me if you want to test my DDES version), but I would very much like to test the DES-SST model but the programming effort is much bigger

About the mix between upwind and central, I read a recent article from Bombardier aerospace (not available yet) where they use the parameter fd (from the Spalart-Allmaras DDES formulation) to blend the schemes. Maybe it would be something to consider since it does not require additional calculation in the model. fd=0 actually forces the RANS mode while fd=1 is equivalent to DES97, and most likely to LES mode. I will try to implement that blending in my DDES-SA model by looking at localBlended scheme as suggested by Fabian, but if you can provide further help for that it would be much appreciated.

Regards,

Philippe
philippebv is offline   Reply With Quote

Old   May 15, 2009, 22:03
Default
  #14
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
Hi Philippe,

Good Morning from China!
1. DDES also includes a low Reynolds number correction, did you notice it?
2. IDDES is really a great idea, a very timely revision to DES concerning LLM. But I lose my idea now about the length scale redefinition, will the cube-root approach violate the IDDES spirit?
3. I'm shocked to find that ANSYS-12.0 has been released with DDES already in it, (even with a option based on SST), sigh... after all, it is Mr. Menter who is working for them with a high frequency activities with DESIDER. You know I once talked to my advisor, boasting that opensource like OpenFOAM is more up-to-date than commercial software, now I realize it is not so always, it depends.

Regards
__________________
~
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   May 16, 2009, 11:56
Default
  #15
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi Philippe,

you can try to add to 'createFields' file something like:

volScalarField localInterface= reinterpret_cast<Foam::incompressible::RASModels:: kOmegaSST_Y*>(turbulence.operator->())->HybInterface();

where HybInterface() is a public member function in your model (in this case "kOmegaSST_Y".

Before the calculation of the momentum equations you would calculate the surfaceScalarField:

Info << "Into UBlending" << endl;
surfaceScalarField surfLocalInterface = fvc::interpolate(localInterface);
surfaceScalarField UBlendingFactor ("UBlendingFactor",surfLocalInterface);

Fabian
braennstroem is offline   Reply With Quote

Old   May 19, 2009, 09:43
Default
  #16
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 didn't know for CFX-12, it's interesting. I think will soon upgrade to CFX-12, so I might be able to test the DDES. But in my opinion, the DES-SST implemented in CFX-11 was already a DDES formulation.

Fabian, thanks for the answer, I'll look into that.

Are any of you going to be at the Workshop in Montreal?
philippebv 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


Similar Threads
Thread Thread Starter Forum Replies Last Post
v2f model implementation for airfoil in FLUENT Sunil FLUENT 2 January 16, 2014 08:15
non-linear k-epsilon model implementation problems Saidi Main CFD Forum 2 March 4, 2010 14:23
DES model in FLUENT Ken FLUENT 2 May 5, 2007 08:07
How to define Epsilon in RSM model? David FLUENT 0 March 17, 2004 10:39
Model and Mesh generation Problems Anindya Main CFD Forum 1 May 19, 2001 02:02


All times are GMT -4. The time now is 02:23.