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

What is the c3 coefficient in k-epsilon model?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 5, 2009, 08:24
Default What is the c3 coefficient in k-epsilon model?
  #1
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hi everyone!

I've tried to find some informations about the coefficients in the k-epsilon turbulence model and i found the c3, a coefficient which I can't find enywhere else. Does anybody know know what is it? And how big should be the value of it? I think the default value is -0.33. Why negative?

Thank's for any help.

Best regards,

Marcin
Marcin is offline   Reply With Quote

Old   June 7, 2009, 16:58
Default
  #2
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
As "mentioned" in the code the default value for c3 is -0.33 and is corresponding to compressible flow only.
It is included in the dissipation equation for epsilon.
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   June 9, 2009, 02:12
Default
  #3
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hallo Sebastian,

thank you for your reply. I have also found these informations in the code. The problem is, I don't uznderstand them. I have comared some equations implemented in OpenFOAM with other, commercial codes (for example CFX) and most of them are simmilar or the same exept for the dissipation equation. I have also compared this equation with some literature and I haven't found anywhere else the C3 coefficient exept for some papers, where the C3 was 0.85. I have also searched for -0.33 value but without success. I would be pleased for some help.

Best regards,

Marcin
Marcin is offline   Reply With Quote

Old   June 9, 2009, 05:59
Default
  #4
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
You habe obviously done far more research on this topic than me.
I'm quite new to turbulence and have only dealt with incompressible fluids so far.
Tough enough without compressible fluids
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   June 10, 2009, 02:11
Default
  #5
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hallo Sebastian,

thak you anyway for your help. All my simulations are compressible and turbulent. The problem is, i have done some simulations of a stator blade of a compressor and comared the results of OpenFOAM with CFX. All values like velocities, pressure, mach number, kinetic energy and temperature of both simulations are quite similar with small or very small differences. The only problematic value is the dissipation. The difference between these codes is quite big with a value between 1e4 and 1e6 in depand of the position. I have no idea what could be the cause. When i change the C3 coefficient from -0.33 to 0.85 it doesn't seem to make a difference in the simulation, but I would anyway like to know, what it is.

Regards,

Marcin
Marcin is offline   Reply With Quote

Old   June 11, 2009, 01:48
Default
  #6
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Marcin

How do you give the inlet boundary value of k and epsilon for you blade?

i am doing the simulation with water pump.it is easy to give a value for SST ,but for k-epsilon,i always get divgence. i tried two ways

1 calculating it from the according the Programme guide P84

2 post the CFX result to get the k and epsilon value

but both leaded to divgence within 100 steps

how can I do

wayne
Quote:
Originally Posted by Marcin View Post
Hallo Sebastian,

thak you anyway for your help. All my simulations are compressible and turbulent. The problem is, i have done some simulations of a stator blade of a compressor and comared the results of OpenFOAM with CFX. All values like velocities, pressure, mach number, kinetic energy and temperature of both simulations are quite similar with small or very small differences. The only problematic value is the dissipation. The difference between these codes is quite big with a value between 1e4 and 1e6 in depand of the position. I have no idea what could be the cause. When i change the C3 coefficient from -0.33 to 0.85 it doesn't seem to make a difference in the simulation, but I would anyway like to know, what it is.

Regards,

Marcin
waynezw0618 is offline   Reply With Quote

Old   June 15, 2009, 02:31
Default
  #7
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Dear Wayne,

I had also problems with the inlet boudary conditions for k and epsilon. I have also tried to set up predetermined values, but it doesn't seem to work in both codes. The one way you can loose it is:

the boudary condition for k:

type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value $internalField;

and for epsilon:

type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005;
value $internalField;

This is also the default adjustment in CFX in inlet. The problem is, that I get with these settings different results for k and epsilon in OpenFOAM and CFX and I don't know where these diffrences come from.
I would be pleased, if you could inform me about your results and how you solve your problem.

Regards, Marcin
Marcin is offline   Reply With Quote

Old   June 16, 2010, 08:39
Default
  #8
New Member
 
Robert
Join Date: Mar 2010
Posts: 16
Rep Power: 7
rob3rt is on a distinguished road
Hi Marcin,

I have a problem with kEpsilonCoeffs. I randomly selected some numbers (i.e. 0.09, 0.14, -0.33, etc.....) and it generates this error:

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon


--> FOAM FATAL ERROR:
Attempt to return primitive entry ITstream : ::kEpsilonCoeffs, line 19, IOstream: Version 2.0, format ASCII, line 0, OPENED, GOOD
primitiveEntry 'kEpsilonCoeffs' comprises
on line 19 the doubleScalar -0.33
as a sub-dictionary

From function const dictionary& primitiveEntry::dict()
in file db/dictionary/primitiveEntry/primitiveEntry.C at line 107.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam:rimitiveEntry::dict() in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#3 Foam::dictionary::subDict(Foam::word const&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 Foam::boussinesq::RASModel::RASModel(Foam::word const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::transportModel&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libboussinesqRASModels.so"
#5 Foam::boussinesq::RASModels::kEpsilon::kEpsilon(Fo am::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::transportModel&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libboussinesqRASModels.so"
#6 Foam::boussinesq::RASModel::adddictionaryConstruct orToTable<Foam::boussinesq::RASModels::kEpsilon>:: New(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::transportModel&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libboussinesqRASModels.so"
#7 Foam::boussinesq::RASModel::New(Foam::GeometricFie ld<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::transportModel&) in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libboussinesqRASModels.so"
#8
in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/my_porousSimpleFoam8"
#9 __libc_start_main in "/lib/libc.so.6"
#10
in "/home/roberto/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/my_porousSimpleFoam8"
Aborted

Do you have any suggestions??

Thanks very much in advance.
rob3rt is offline   Reply With Quote

Old   January 16, 2011, 11:18
Default compressible Launder Sharma k-e model
  #9
New Member
 
Dmitry
Join Date: Jan 2011
Posts: 2
Rep Power: 0
DimaZ is on a distinguished road
Hi all,
Does anybody know the reference for the implementation of the compressible k-e Launder Sharma k-epsilon model in OpenFOAM?
The incompressible formulation follows: Launder, B. E. and Sharma, B. I. (1974), "Application of the Energy-Dissipation Model of Turbulence to the Calculation of Flow Near a Spinning Disc", Letters in Heat and Mass Transfer, Vol. 1, No. 2, pp. 131-138.

But in the compressible implementation there is the constant CEpsilon3 and I'm just wondering about the reference for it.

Thanks in advance,
Dmitry

DimaZ is offline   Reply With Quote

Old   July 1, 2011, 09:06
Default
  #10
Member
 
The True
Join Date: Dec 2010
Posts: 80
Rep Power: 6
Eren10 is on a distinguished road
Quote:
Originally Posted by DimaZ View Post


But in the compressible implementation there is the constant CEpsilon3 and I'm just wondering about the reference for it.


I want to use the incompressible case, but I see also there a C3 -0.33; I can't see this value in the paper of Launder ans Sharma. Did they introduced this term later ?

And is there a tutorial of LaunderSharma ? I want to see the required files.

Thanks.
Eren10 is offline   Reply With Quote

Old   July 4, 2011, 03:37
Default
  #11
New Member
 
Dmitry
Join Date: Jan 2011
Posts: 2
Rep Power: 0
DimaZ is on a distinguished road
Quote:
Originally Posted by Eren10 View Post
I want to use the incompressible case, but I see also there a C3 -0.33; I can't see this value in the paper of Launder ans Sharma. Did they introduced this term later ?

And is there a tutorial of LaunderSharma ? I want to see the required files.

Thanks.
I did not find any. Regarding the tutorials and files: I can send you one of my own test cases, witch are validated, documented and published.
Best regards,
Dmitry
DimaZ is offline   Reply With Quote

Old   July 19, 2013, 04:48
Default Need some explanation on kEpsilon.C
  #12
New Member
 
RJ HO
Join Date: Dec 2012
Posts: 21
Rep Power: 4
RJ87 is on a distinguished road
Hi foamers,

I check through kEpsilon.C file and don't quite understand how

Code:
 tmp<fvScalarMatrix> epsEqn
    (
        fvm::ddt(rho_, epsilon_)
      + fvm::div(phi_, epsilon_)
      - fvm::Sp(fvc::ddt(rho_) + fvc::div(phi_), epsilon_)
      - fvm::laplacian(DepsilonEff(), epsilon_)
     ==
        C1_*G*epsilon_/k_
      - fvm::SuSp(((2.0/3.0)*C1_ + C3_)*rho_*divU, epsilon_)
      - fvm::Sp(C2_*rho_*epsilon_/k_, epsilon_)
    );
why is the dissipative term is (- fvm::SuSp(((2.0/3.0)*C1_ + C3_)*rho_*divU, epsilon_)) instead of (- fvm::SuSp(((2.0/3.0)*C1_ - C3_)*rho_*divU, epsilon_).

I look through turbulence papers indicating that usage -((2.0/3.0)*C1-C3) with C3 assigned with negative value between 0 to 1 with the whole dissipative term a negative value. OpenFoam -((2.0/3.0)*C1+C3) with constant C3 assign with negative value of -0.33. In this case, if C3 is large enough, dissipative term will be a positive value. Any chances that something is wrong with the codes?
RJ87 is offline   Reply With Quote

Old   June 12, 2014, 01:33
Default
  #13
Member
 
Fabian E.
Join Date: Nov 2009
Posts: 36
Rep Power: 7
galap is on a distinguished road
I have a question which goes in the same direction. Why is actually in the compressible kEpsilon model equation the constant C3 included in this way? For me, I don't understand why C3 contributes to the reynolds shear stress term, which does not follow the standard formulation according to

http://www.cfd-online.com/Wiki/Standard_k-epsilon_model

or books from e.g. Pope and Poisnot

C3 should be the constant for source due to buoyancy.


tmp<fvScalarMatrix> epsEqn
(
fvm::ddt(rho_, epsilon_)
+ fvm::div(phi_, epsilon_)
- fvm::Sp(fvc::ddt(rho_) + fvc::div(phi_), epsilon_)
- fvm::laplacian(DepsilonEff(), epsilon_)
==
C1_*G*epsilon_/k_
- fvm::SuSp(((2.0/3.0)*C1_ + C3_)*rho_*divU, epsilon_)
- fvm::Sp(C2_*rho_*epsilon_/k_, epsilon_)
);

I would exspect something like

..
- fvm::SuSp(((2.0/3.0)*C1_)*rho_*divU, epsilon_) + C3_*(..)
..
galap is offline   Reply With Quote

Old   December 16, 2014, 07:07
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

Quote:
Originally Posted by Marcin View Post
I've tried to find some informations about the coefficients in the k-epsilon turbulence model and i found the c3, a coefficient which I can't find enywhere else. Does anybody know know what is it?
Sorry for the necro-bump, but the CFD-Online forums follow the principle of using a thread on the same topic to keep things on-topic, and there are some news about this question:
Just in case something happens to the internet, the reference added was this one:
Code:
    Reference:
        "k-epsilon equations for compressible reciprocating engine flows"
        El Tahry, S. H.,
        AIAA Journal of Energy 7 (1983), 345-353.
Best regards,
Bruno
wyldckat 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
Reynolds Stress model in CFX vs Fluent Tim CFX 1 October 7, 2009 06:19
Simulation of a single bubble with a VOF-method Suzzn CFX 18 October 2, 2009 04:18
No results for solid domain Gary Holland CFX 10 March 13, 2009 04:30
Steam Diffusion Coefficient - Mixture model Graham Brett FLUENT 0 February 21, 2008 18:32
Reflection coefficient of particle in DPM model S.J.R FLUENT 1 June 9, 2007 19:03


All times are GMT -4. The time now is 14:11.