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

Missing Term in RAS-Models

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

Like Tree2Likes
  • 2 Post By alberto

Reply
 
LinkBack Thread Tools Display Modes
Old   June 15, 2010, 07:16
Default Missing Term in RAS-Models
  #1
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi all

There is a missing term in the RAS-model implementation in OpenFOAM 1.5.x, 1.5-dev and 1.6.x. This term is at least missing in the

kOmega (only present in 1.6.x)
kOmegaSST
kEpsilon

models. The problem is with the function

Code:
tmp<fvVectorMatrix> kOmega::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(fvc::grad(U)().T()))
    );
}
which should take the form

Code:
tmp<fvVectorMatrix> kOmega::divDevReff(volVectorField& U) const
{
    return
    (
      - fvm::laplacian(nuEff(), U)
      - fvc::div(nuEff()*dev(fvc::grad(U)().T()))
      + 2.0 / 3.0 * fvc::grad(k_)
    );
}
This additional term, [ 2.0 / 3.0 * fvc::grad(k_) ], cause a driving force due to gradients in the normal part of the Reynold's stress tensor.

The other turbulence models might be affected as well, however as I am unfamiliar with those, I have not looked into the implementation.

Best regards,

Niels

P.S. My colleagues has done some preliminary tests and it seems that having this contribution co-aligned with the pressure gradients does not affect the results, however if they are perpendicular, the gradient in the normal Reynold's stresses is the only driving force.
ngj is offline   Reply With Quote

Old   July 7, 2010, 08:13
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Bump.

I can see that this term has not been included in the new 1.7.0 release. Any comments on post #1?

Cheers,

Niels
ngj is offline   Reply With Quote

Old   July 9, 2010, 14:55
Default intersting but simple answer
  #3
New Member
 
parham momeni
Join Date: Mar 2009
Location: glasgow, uk
Posts: 25
Rep Power: 7
mcjicpm2 is an unknown quantity at this point
It is correct since the pressure in the simple scheme is relative so it has no affect on the integration on both side of the control volume this source term will disapear, It is correct
mcjicpm2 is offline   Reply With Quote

Old   July 15, 2010, 04:56
Default
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Parham

I do not quite follow you. If there is a gradient in the turbulence, then there must be a driving force and this force is not included into the present releases of OpenFOAM, hence the term is important for specific purposes and needs to be included.

It has nothing to do with the simple-algorithm, as it is a more general bug inside the turbulence models.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   July 15, 2010, 05:17
Default
  #5
New Member
 
parham momeni
Join Date: Mar 2009
Location: glasgow, uk
Posts: 25
Rep Power: 7
mcjicpm2 is an unknown quantity at this point
Hi, the pressure in the code is relative isnt it? so if you add or remove -2/3k from or to it, it realy doesnt matter. I have seen this in other codes. since in the simple algorhm the pressure is relative pressure so p- or + any thing lets say 2/3 k should not matter.
mcjicpm2 is offline   Reply With Quote

Old   July 15, 2010, 05:57
Default
  #6
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi

You assume that k is constant, however as it is not, fvc::grad(k) results in a driving force.

We have verified that without this term experimental data cannot be reproduced under certain conditions, however including it yield good correlation between data and model.

The term comes from the Boussinesq approximation of the Reynolds stress tensor, hence the RANS formulation is incomplete due to its omission.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   July 16, 2010, 07:35
Default
  #7
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
I agree with you. The 2/3 * k IS included in the UEqns.H file for bubbleFoam/twoPhaseEulerFoam which are the codes I use the most.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   July 16, 2010, 08:14
Default
  #8
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Laurence

I see, I had not thought of looking into the individual solvers. However both simpleFoam and turbFoam uses divDevReff, however those could off course be changed instead.

Have a nice weekend,

Niels
ngj is offline   Reply With Quote

Old   July 16, 2010, 09:09
Default
  #9
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
Also, shouldn't 'dev' actually be 'dev2' in divDevReff.

This is confusing me a lot now. . I will try deriving the implementation from the theory over the weekend if I have time.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   August 4, 2010, 17:15
Default
  #10
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
Do you have a copy of Turbulent Flows by Pope? Page 93 explains how the pressure, p, is modified to p + 2/3 k.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   August 5, 2010, 05:05
Default
  #11
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Laurence

Unfortunately not, however would it be possible for you to email me the relevant page?

Best regards,

Niels
ngj is offline   Reply With Quote

Old   March 16, 2011, 01:23
Default
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi,

you can simply re-write grad(p + 2/3k) = grad(p*). This will lead to a solution algorithm which is identical to what is implemented in OpenFOAM incompressible solvers.

@Laurence: in bubbleFoam/twoPhaseEulerFoam k is included in the fluid phase independently in each phase because its effect is different on each phase. In phase a there is the Ct coefficient. Notice also that you find the pressure gradient from the total continuity, and each phase has it scaled only by the corresponding phase fraction.

Best,
JinBiao and fumiya like this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   March 16, 2011, 05:14
Default
  #13
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
Thanks Alberto, we continued by email, apologies for leaving the thread dangling!

When would you (or anyone) alter the C_t coefficient, and do you know of any published material that has ever done that? I vaguely recall reading a paper where they did but I can't find it (if I could give 2 pieces of advice to anyone starting a cfd project, it would be BACKUP and organise your literature!).
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   March 16, 2011, 19:28
Default
  #14
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi Laurence,

Ct should be related to the time scale of turbulence interaction between particles/bubbles and fluid turbulent structure. I do not remember where I saw this model tested changing Ct. First thing that comes to my mind is H. Rusche thesis however.

Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 14, 2011, 08:04
Default
  #15
New Member
 
Andreas Herwig
Join Date: Jan 2011
Posts: 6
Rep Power: 6
Andreas.Herwig is on a distinguished road
Quote:
Originally Posted by alberto View Post
Hi,

you can simply re-write grad(p + 2/3k) = grad(p*). This will lead to a solution algorithm which is identical to what is implemented in OpenFOAM incompressible solvers.

@Laurence: in bubbleFoam/twoPhaseEulerFoam k is included in the fluid phase independently in each phase because its effect is different on each phase. In phase a there is the Ct coefficient. Notice also that you find the pressure gradient from the total continuity, and each phase has it scaled only by the corresponding phase fraction.

Best,
Hi,

I'm already searching a long time where this modified pressure is calculated grad(p + 2/3k) = grad(p*) in pisoFoam or the kEpsilon Code but can't find it. So if anyone knows ...

Thanks a lot.

Andreas
Andreas.Herwig is offline   Reply With Quote

Old   April 14, 2011, 17:19
Default
  #16
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by Andreas.Herwig View Post
Hi,

I'm already searching a long time where this modified pressure is calculated grad(p + 2/3k) = grad(p*) in pisoFoam or the kEpsilon Code but can't find it. So if anyone knows ...

Thanks a lot.

Andreas
If you write your momentum equation as a function of p*, and derive the pressure equation directly, you will find out that you do not have to do that calculation in the case of incompressible flows ;-)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   February 27, 2012, 12:26
Default
  #17
Member
 
AleDR's Avatar
 
Alessandro
Join Date: May 2009
Location: Genova
Posts: 43
Rep Power: 8
AleDR is on a distinguished road
Dear Foamers,

Sorry for reopening this thread, but I still can't understand the point...

Ok for rewriting grad(p/rho + 2/3*k) as grad(p_*) in the momentum equation, but what about boundary conditions?

As a consequence of the pseudo-pressure formulation in /0 it will be specified one b.c. for p_* (not p) and one for k (which is part of p_*). Is this generally acceptable?

Moreover from what I see at first sight in /compressible/RAS/kEpsilon this formulation still holds for the term divDevRhoReff... will this mean that p used in perfectGas is p*=p + 2/3*k ?

I am really confused about the matter...


Thanks for any help!

.A.
AleDR is offline   Reply With Quote

Old   February 29, 2012, 08:05
Question
  #18
Member
 
AleDR's Avatar
 
Alessandro
Join Date: May 2009
Location: Genova
Posts: 43
Rep Power: 8
AleDR is on a distinguished road
Hints? Suggestions? References?

...or maybe it's a silly question?

.A.
AleDR 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
Numerical Problems with Non-Linear RAS models cfdmarkus OpenFOAM Running, Solving & CFD 1 August 18, 2015 05:48
Turbulence dampening due to magnetic field in LES and RAS eelcovv OpenFOAM 0 June 8, 2010 11:35
RAS Turbulence Models - Convective Term john_w OpenFOAM 3 May 29, 2010 21:31
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
wall functions for RAS models Epf OpenFOAM Pre-Processing 3 April 8, 2010 11:14


All times are GMT -4. The time now is 23:54.