CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Bugs

Possible Incompressible Turbulence Model Bugs

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 2, 2009, 13:55
Default Possible Incompressible Turbulence Model Bugs
  #1
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
I've been evaluating the OpenFOAM 1.6.x incompressible turbulence models and came across possible bugs/anomalies, though they could also be due to my limited understanding.

My test case was a simple cube with 4 walls, an inlet and an opposing outlet.

The following models worked as I'd expect:
kEpsilon, laminar, RNGkEpsilon, SpalartAllmaras, LRR, LaunderGibsonRSTM, LienCubicKE, qZeta, LienCubicKELowRe, kOmegaSST

The following models had problems:

1) Foam::incompressible::RASModels::NonlinearKEShih

Issues error:

kqRWallFunction is the wrong k patchField type for wall-functions on patch face_2
should be zeroGradient

From function wall-function evaluation
in file OpenFOAM-1.6.x/src/finiteVolume/lnInclude/checkPatchFieldTypes.H at line 3.

Where face_2 is a wall - is this a special model that uses zeroGradient on a wall instead of kqRWallFunction?

2) Foam::incompressible::RASModels::LaunderSharmaKE

Issues warning:

--> Creating nut to employ run-time selectable wall functions
Writing new nut

Supposed to be low-Re model so doesn't use wall functions.

3) Foam::incompressible::RASModels::LamBremhorstKE

Should be low-Re (I think?), but seems to auto-correct k, epsilon, and adds nut as if wall function model, then runs successfully.

Also issues warning:

--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/rjs/projects/of/of1.6/OpenFOAM-1.6.x/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field epsilon would be more appropriate.

4) Foam::incompressible::RASModels::LienLeschzinerLowRe

Always fails for same standard case as I've used, successfully, for all other turbulence models.

Solution fails:

DILUPBiCG: Solving for k: solution singularity

Anybody else seeing these issues?
__________________
Symscape, Computational Fluid Dynamics for all
gocarts is offline   Reply With Quote

Old   September 4, 2009, 05:55
Default
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Thanks. We pushed some fixes to the incompressible turbulence models in 1.6.x It all should work now as intended.
mattijs is offline   Reply With Quote

Old   September 11, 2009, 18:28
Default Might be more
  #3
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
Good work mattijs,

I checked the incompressible low-Re incompressible RAS models I mentioned in my previous post and they now seem fine, except for Foam::incompressible::RASModels::LienLeschzinerLowRe - which although I can get it to converge, it still seems sensitive to k values derived from turbulent intensity > 0.01.

I guess too that zeroGradient is the right condition for a wall, where I'd expected kqRWallFunction, for Foam::incompressible::RASModels::NonlinearKEShih?

The compressible RAS Turbulence models I tested:
kEpsilon, RNGkEpsilon, SpalartAllmaras, realizableKE, LaunderSharmaKE, LRR, LaunderGibsonRSTM, kOmegaSST

all seemed fine except for:
Foam::compressible::RASModels::LaunderSharmaKE

which failed with the error:
NO_READ specified for read-constructor of object k of class IOobject

The traceback pointed to the constructor:
Foam::compressible::RASModels::LaunderSharmaKE::La underSharmaKE

Again some of these issues could well be related to my lack of understanding.
__________________
Symscape, Computational Fluid Dynamics for all
gocarts is offline   Reply With Quote

Old   September 14, 2009, 13:11
Default
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Thanks. We pushed (to 1.6.x) a fix for the LaunderSharmaKE. The non-linear k-eps hasn't been converted yet to the new 'boundary conditions on nut' treatment so uses the old zero-gradient method.

Thanks for reporting,

Mattijs
mattijs is offline   Reply With Quote

Old   September 14, 2009, 21:20
Default Thanks
  #5
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
Hi Mattijs,

Thanks for the update, great work from the OpenCFD team.
__________________
Symscape, Computational Fluid Dynamics for all
gocarts is offline   Reply With Quote

Old   November 24, 2009, 14:55
Default
  #6
Member
 
Sven Schweikert
Join Date: Jun 2009
Posts: 38
Rep Power: 7
svens is on a distinguished road
Hi Richard

For me it seems to be that you are really delved into OpenFOAMs incompressible RAS models.

I was running some calculation with the LaunderGibsonRSTM and the kEpsilon models. It was a little bit surprising that the RSTM performs really poor compared to the EVM. (I simulated a u-duct geometry.)

It would be nice to her from you about your experiences with the different turbulence models - and of course especially about the RSTMs. Did they perform satisfactorily? Any problems to reach this state?

Thanks pretty much
Sven
svens is offline   Reply With Quote

Old   November 24, 2009, 16:51
Default Initial Velocity Sensitivity
  #7
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
Hi Sven,

I haven't performed detailed comparisons between the turbulence models. However, for a internal flow calculation using simpleFoam (steady-state) I noticed that the Launder Gibson RSTM was sensitive to the initial velocity condition. I found that whereas the k-epsilon could be initialized with the inlet velocity, the LG RSTM preferred zero.

Hope this helps.

Edit: For the same simple case the LG RSTM calculation took twice as many iterations as the K-E calculation to reach a steady state.
__________________
Symscape, Computational Fluid Dynamics for all

Last edited by gocarts; November 24, 2009 at 16:57. Reason: Added details
gocarts is offline   Reply With Quote

Old   November 24, 2009, 19:08
Default
  #8
Member
 
Sven Schweikert
Join Date: Jun 2009
Posts: 38
Rep Power: 7
svens is on a distinguished road
Thanks Richard

I'm using a converged k-epsilon solution as initials for the RSTM - this leads to satisfactorily behavior in convergence. But as mentioned the comparistion to experimental data and EVM shows not the hoped improvement...

I mean - I'm using a 180deg u-duct - a geometry with strong streamline curvature. I thought on problems like this the RSTMs turn to account!

Do you have some experiences with the fvSchemes? I'm using a lot of 1st order (standard simpleFoam settings) schemes and I'm quite unsure what they should be for RSTMs.

Thank you very much
Sven
svens is offline   Reply With Quote

Old   November 24, 2009, 21:28
Default
  #9
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
Yes, I believe you are right u-bends are RSM territory.

My experience with fvSchemes isn't extensive. However, the div scheme settings are critical in determining accuracy - if you are using the default settings from a simpleFoam tutorial (likely upwind) then consider trying (2nd order) linearUpwind for your scalars and linearUpwindV for vectors (i.e., velocity).

Other variables to consider are the mesh density and whether your y+ values are within the log-law limit range - I'm guessing that you are happy with these.

I'm also assuming that you are confident that your boundary conditions (especially at the inlet) are valid for R - likely derived from k.
__________________
Symscape, Computational Fluid Dynamics for all
gocarts is offline   Reply With Quote

Old   November 25, 2009, 15:22
Default
  #10
Member
 
Sven Schweikert
Join Date: Jun 2009
Posts: 38
Rep Power: 7
svens is on a distinguished road
Thanks for your reply Richard

I just had a look at an evaluation for a finer grid - the values becoming better!

At the moment I'm experimenting with the 'nNonOrthogonalCorrectors' which hopefully also leads to a more reasonable result. As soon as I figured out these influences I'm going to have a run with 2nd order discretication schemes.

Time and cpu resource is rare - does it make sense to restart a already converged simulation with higher fvSchemes or do I have to start from 0 again? A question which bothers me...

Thanks again Richard you are providing me great support.
Sven
svens is offline   Reply With Quote

Old   November 25, 2009, 17:00
Default 1st vs 2nd Order RSTM
  #11
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
I've found starting each from scratch to produce the fastest convergence rate.

So when I say try 2nd order I mean for the velocity and pressure. I haven't tried 2nd order for the turbulent variables. I have something like:

Code:
divSchemes
{
    default         Gauss linearUpwind Gauss linear;
    div(phi,U)      Gauss linearUpwindV Gauss linear;
    div((nuEff*dev(grad(U).T()))) Gauss linear;

    div(phi,k) Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div(phi,R) Gauss upwind;
    div(R) Gauss linear; 
    div((mu*dev2(grad(U).T()))) Gauss linear; 
    div((rho*R)) Gauss linear;
}
Attached is a comparison on the same relatively coarse grid of Launder Gibson RSTM 1st vs 2nd order - as you can see there are significant differences downstream of the bend.
Attached Images
File Type: png 1st-vs-2nd-order.png (80.4 KB, 101 views)
__________________
Symscape, Computational Fluid Dynamics for all
gocarts is offline   Reply With Quote

Old   November 25, 2009, 18:34
Default
  #12
Member
 
Sven Schweikert
Join Date: Jun 2009
Posts: 38
Rep Power: 7
svens is on a distinguished road
Hey Richard - that's amazing! Thanks for your illustration.

Another little question to understand completely - you'r using
Code:
  div(phi,U)      Gauss linearUpwindV Gauss linear;
How can I understand the usage of 2 times a discretisation and interpolation scheme? Is one for phi and the other for U?

Thank you very much for great help!
Sven
svens is offline   Reply With Quote

Old   November 26, 2009, 15:58
Default div upwindLinearV scheme requires grad scheme
  #13
Senior Member
 
gocarts's Avatar
 
Richard Smith
Join Date: Mar 2009
Location: Enfield, NH, USA
Posts: 138
Blog Entries: 4
Rep Power: 7
gocarts is on a distinguished road
For div the upwindLinearV (vector) scheme is special in that it also requires a grad scheme hence the addition of 'Gauss Linear'. You don't need to specify a grad scheme for upwindLinear (scalar) - so my inclusion of it in my sample code is ignored by OpenFOAM.

Again I can't claim to be an expert in these matters. I came across this case by trial and error. For instance if you don't specify a grad scheme for upwindLinearV you'll receive the following error:

Code:
--> FOAM FATAL IO ERROR: 
Grad scheme not specified

Valid grad schemes are :

8
(
fourth
cellMDLimited
Gauss
cellLimited
faceMDLimited
faceLimited
extendedLeastSquares
leastSquares
)
__________________
Symscape, Computational Fluid Dynamics for all
gocarts 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
Adding a Turbulence Model doug OpenFOAM Running, Solving & CFD 10 October 2, 2012 07:55
Eul-Eul flow, k-e-kp-ep-Theta Turbulence model us FLUENT 5 April 5, 2011 03:29
What is advection term of incompressible turbulence model waynezw0618 OpenFOAM Running, Solving & CFD 2 December 6, 2008 08:46
Turbulence Model GG CD-adapco 3 March 3, 2008 20:06
SSG Reynolds Turbulence Model Georges CFX 1 February 28, 2007 17:15


All times are GMT -4. The time now is 10:28.