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

error on turbulence scheme

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

Like Tree3Likes
  • 1 Post By Tobi
  • 1 Post By wyldckat
  • 1 Post By s.m

Reply
 
LinkBack Thread Tools Display Modes
Old   May 27, 2013, 06:17
Default error on turbulence scheme
  #1
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
Hi
I set a second order turbulence scheme with an error:
Code:
divSchemes
{
    default none;
    div(tauMC) Gauss linear;
    div(phi) Gauss linearUpwindV;
    div(phi,omega) Gauss upwind;
    div(phi,k) Gauss linearUpwind;
    div(phi,gas) Gauss limitedLimitedLinear 1 0 1;
    div(phi,epsilon) Gauss linearUpwind;
}
Code:
--> FOAM Warning :
From function polyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 474
Patch empty specifies a group empty which is also a patch name. This might give problems later on.
Reading field U

Reading field gas

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model realizableKE
realizableKECoeffs
{
Cmu             0.09;
A0              4;
C2              1.9;
sigmak          1;
sigmaEps        1.2;
Prt             1;
}

fluxScheme: Kurganov

Starting time loop

Mean and max Courant Numbers = 3.858134887 23.51635184
deltaT = 2.083333333e-09
Time = 2.08333e-09

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
[0] swak4Foam: Allocating new repository for sampledGlobalVariables
[1] swak4Foam: Allocating new repository for sampledGlobalVariables
[2] swak4Foam: Allocating new repository for sampledGlobalVariables
[3] swak4Foam: Allocating new repository for sampledGlobalVariables
smoothSolver:  Solving for Ux, Initial residual = 0.999875462, Final residual = 1.076653513e-16, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 7.204656079e-17, No Iterations 2
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for h, Initial residual = 2.679038313e-06, Final residual = 5.013352019e-08, No Iterations 2
time step continuity errors : sum local = 0, global = 0, cumulative = 0
[0]
[0]
[0] --> FOAM FATAL IO ERROR:
[0] attempt to read beyond EOF
[0]
[0] file: /home/ehsan/Desktop/Central/nonUniformMesh/test2/processor0/../system/fvSchemes.divSchemes.div(phi,epsilon) at line [3] [1]
[2]
[2] 61.
[0]
[0]     From function ITstream::read(token&)
[0]     in file db/IOstreams/Tstreams/ITstream.C at line 83.
[0]
FOAM parallel run exiting
[0]
[1]
[1] --> FOAM FATAL IO ERROR:
[1] attempt to read beyond EOF
[1]
[1] file: IOstream.divSchemes.div(phi,epsilon) at line 0
[2] --> FOAM FATAL IO ERROR:
[2] attempt to read beyond EOF
[2] .
[1]
[1]     From function ITstream::read(token&)
[1]     in file db/IOstreams/Tstreams/ITstream.C at line 83.
[1]
FOAM parallel run exiting
[1]

[3]
[3] --> FOAM FATAL IO ERROR:
[3] attempt to read beyond EOF
[3]
[3] file: IOstream.divSchemes.div(phi,epsilon) at line 0.
[3]
[3]     From function ITstream::read(token&)
[3]     in file db/IOstreams/Tstreams/ITstream.C at line 83.
[3]
FOAM parallel run exiting
[3]

[2] file: IOstream.divSchemes.div(phi,epsilon) at line 0.
[2]
[2]     From function ITstream::read(token&)
[2]     in file db/IOstreams/Tstreams/ITstream.C at line 83.
[2]
FOAM parallel run exiting
[2]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 2 in communicator MPI_COMM_WORLD
with errorcode 1.

NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
--------------------------------------------------------------------------
--------------------------------------------------------------------------
mpirun has exited due to process rank 1 with PID 11063 on
node Ehsan-com exiting without calling "finalize". This may
have caused other processes in the application to be
terminated by signals sent by mpirun (as reported here).
--------------------------------------------------------------------------
[Ehsan-com:11055] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
[Ehsan-com:11055] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
Killing PID 11052
 PyFoam WARNING on line 232 of file /usr/local/lib/python2.7/dist-packages/PyFoam/Execution/FoamThread.py : Process 11052 was already dead
I like to know experiments about which scheme(preferably second order) is more appropriate (stable and accurate with physical results) for k,omega and epsilon?
thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   May 27, 2013, 08:21
Default
  #2
New Member
 
bscphil's Avatar
 
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5
bscphil is on a distinguished road
Quote:
Originally Posted by immortality View Post
Hi
I set a second order turbulence scheme with an error:
Code:
divSchemes
{
    default none;
    div(tauMC) Gauss linear;
    div(phi) Gauss linearUpwindV;
    div(phi,omega) Gauss upwind;
    div(phi,k) Gauss linearUpwind;
    div(phi,gas) Gauss limitedLimitedLinear 1 0 1;
    div(phi,epsilon) Gauss linearUpwind;
}
Hi,
the question to me is, which version of OpenFoam you are using (the syntax is different in different versions) ?

In OpenFoam 2.2.0 just do:
Code:
divSchemes
{
default                     none;
div(phi,U)                  bounded Gauss linearUpwindV grad(U);
div(phi,k)                  bounded Gauss linearUpwind grad(k);
div(phi,omega)                 bounded Gauss linearUpwind grad(omega);
}
for a k-omega turbulence model and second order upwind schemes for the divergence terms.
bscphil is offline   Reply With Quote

Old   May 27, 2013, 12:33
Default
  #3
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
thanks Philip
yes,I use version 2.2.0
now I'm using rhoCentralFoam and it doesn't have a div(phi,U) in it.
what to do with div(phi) instead?
my case is unsteady and compressible.
when we have to use bounded keyword?what conditions the problem should have?
thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   May 27, 2013, 16:50
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

@Ehsan: "bounded" is the default option that OpenFOAM 2.2 indicates it will use, if not present in the respective line.
For more information on this characteristic, see section "4.4.2 Surface normal gradient schemes" on the User Guide.
Personally, I have no clue when "bounded" or other methods should be used... But the descriptions shown in the User Guide seem self-explanatory!?

And as Phillip hinted, the problem you were having was the missing "grad(epsilon)":
Code:
div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon);
As for "div(phi)": if when you remove the respective line, the solver doesn't complain, then it's because it's not even used by the solver (because you have "default none;").

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   June 2, 2013, 02:19
Default
  #5
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
thanks.
You mean 'bounded' is related to snGrad ?or may be different to that?
I removed div(phi) without OF complaining.
Then OF uses a default method for this term in rhoCentralFoam?
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   June 9, 2013, 10:15
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by immortality View Post
I removed div(phi) without OF complaining.
Then OF uses a default method for this term in rhoCentralFoam?
I can only assume that "div(phi)" is simply not calculated, because of the "default none;" entry in "divSchemes".

Quote:
Originally Posted by immortality View Post
You mean 'bounded' is related to snGrad ?or may be different to that?
Well, apparently there are a few usages of the "bounded" word going around in OpenFOAM's source code I only mentioned the ones I found in the User Guide, which referred to the surface gradients...

But after looking at the source code, here's what I found:
  • From the file "src/finiteVolume/finiteVolume/convectionSchemes/boundedConvectionScheme/boundedConvectionScheme.H"

    Quote:
    Bounded form of the selected convection scheme.

    Boundedness is achieved by subtracting div(phi)*vf or Sp(div(phi), vf)
    which is non-conservative if div(phi) != 0 but conservative otherwise.

    Can be used for convection of bounded scalar properties in steady-state
    solvers to improve stability if insufficient convergence of the pressure
    equation causes temporary divergence of the flux field.
  • There are a few other files that mention the word "bounded", but seem to be unrelated to this one above.
wyldckat is offline   Reply With Quote

Old   June 9, 2013, 11:37
Default
  #7
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
thanks.
so bounded schemes can be only used in steady-state runs as i have understood.
many thanks.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   June 9, 2013, 12:24
Default
  #8
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,077
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,

you can use the bounded scheme in non steady-state cases too.

http://www.openfoam.org/version2.2.0/numerics.php

The functionallity of that scheme is defined in the libOpenSmoke thread.
wyldckat likes this.
Tobi is offline   Reply With Quote

Old   June 9, 2013, 13:07
Default
  #9
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
yes I forgot about that thread.but I yet don't know exactly when bounded scheme should be used.
my case is compressible and unsteady and haven't a convergence problem.
then should I use bounded?
the fvScheme I use is this,is it correct or which changes I have to do?
Code:
fluxScheme      Kurganov;

ddtSchemes
{
    default         CrankNicolson .5;
    //ddt(rho)        CrankNicolson .5;
    //ddt(rhoU)       CrankNicolson .5;
    //ddt(rhoE)       Euler;
    //ddt(rho,U)      Euler;
    //ddt(rho,e)      Euler;
    //ddt(rho,h)      Euler;
    //ddt(rho,omega)  Euler;
    //ddt(rho,k)      Euler;
    //ddt(rho,gas)    Euler;
}

gradSchemes
{
    default         none;
    grad(U) Gauss linear;
    grad(rho) Gauss linear;
    grad(rhoU) Gauss linear;
    grad((1|psi)) Gauss linear;
    grad(e) Gauss linear;
    grad((1|thermo:psi)) Gauss linear;
    grad(h) Gauss linear;
    grad(sqrt(((Cp|Cv)*(1|psi)))) Gauss linear;
    grad(sqrt(((Cp|Cv)*(1|thermo:psi)))) Gauss linear;
    grad(T) Gauss linear;
    grad(omega) cellMDLimited Gauss linear 1;
    grad(k) cellMDLimited Gauss linear 1;
    grad(gas) Gauss linear;
    grad(epsilon) Gauss linear;
}

divSchemes
{
    default none;
    div(tauMC) Gauss linear;
    div(phi) bounded Gauss linearUpwindV;
    div(phi,omega) bounded Gauss linearUpwind grad(omega);
    div(phi,k) bounded Gauss linearUpwind grad(k);
    div(phi,gas) Gauss limitedLimitedLinear 1 0 1;
    div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon);
}

laplacianSchemes
{
    default         none;
    laplacian(muEff,U) Gauss linear corrected;
    laplacian(alphaEff,e) Gauss linear corrected;
    laplacian(alpha,e) Gauss linear corrected;
    laplacian(k,T) Gauss linear corrected;
    laplacian(DepsilonEff,omega) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DomegaEff,omega) Gauss linear corrected;
    laplacian(alphaEff,h) Gauss linear corrected;
    laplacian(muEff,gas) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
}

interpolationSchemes
{
    default none;
    reconstruct(rho) vanLeer;
    reconstruct(U) vanLeerV;
    reconstruct(T) vanLeer;
    interpolate(rho) linear;
    interpolate(U) linear;
    interpolate(rhoU) linear;
    interpolate(muEff) linear;
    interpolate(tauMC) linear;
}

snGradSchemes
{
    default none;

    snGrad(U) corrected;

}
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality is offline   Reply With Quote

Old   August 20, 2013, 06:57
Default
  #10
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
hi
can any one explian that what is the definition of bounded and unbounded schemes, e.g in this table for explain behaviour of interpolation schemes,
which one is better, bounded or unbounded schemes?


Table 4.10. Behaviour of interpolation schemes used in divSchemes
linear : Second order, unbounded
skewLinear : Second order, (more) unbounded, skewness correction
cubicCorrected : Fourth order, unbounded
upwind : First order, bounded
linearUpwind : First/second order, bounded
QUICK : First/second order, bounded
TVD schemes : First/second order, bounded
SFCD : Second order, bounded
NVD schemes : First/second order, bounded
s.m is offline   Reply With Quote

Old   August 21, 2013, 06:51
Default
  #11
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Saeideh,

You can find some notions of what "bounded" is on the Programmers Guide: http://foam.sourceforge.net/docs/Gui...mmersGuide.pdf
Some more mentions are here: http://www.cfd-online.com/Wiki/Appro...grids_-_Common

From the following link - http://cfd.mace.manchester.ac.uk/twi...s/cfd1-pt1.pdf - I quote:
Quote:
Originally Posted by http://cfd.mace.manchester.ac.uk/twiki/pub/Main/TimCraftNotes_All_Access/cfd1-pt1.pdf
Boundedness
  • Ensures that the numerical solution lies within physical bounds.
  • For example, in a heat conduction problem the minimum and maximum temperatures should occur on the domain boundaries. A bounded scheme would not produce spurious maxima/minima within the domain.
  • Higher order discretization schemes (which one might want to use for accuracy) can often produce unbounded solutions in the form of undershoots and overshoots, which can sometimes lead to stability and convergence problems.
Best regards,
Bruno
immortality likes this.
wyldckat is offline   Reply With Quote

Old   August 21, 2013, 08:45
Default
  #12
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 5
s.m is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Hi Saeideh,

You can find some notions of what "bounded" is on the Programmers Guide: http://foam.sourceforge.net/docs/Gui...mmersGuide.pdf
Some more mentions are here: http://www.cfd-online.com/Wiki/Appro...grids_-_Common

From the following link - http://cfd.mace.manchester.ac.uk/twi...s/cfd1-pt1.pdf - I quote:


Best regards,
Bruno
Thank you very Much, they were too usefull.
immortality likes this.
s.m 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
Wrong calculation of nut in the kOmegaSST turbulence model FelixL OpenFOAM Bugs 27 March 27, 2012 09:02
how to understand high resolution scheme and high order scheme iilw1314 Main CFD Forum 3 September 30, 2010 10:43
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 20:28
Analyze Turbulence Camilo Costa CFX 7 December 4, 2006 12:00
Stabilizing turbulence equation in channel flow Biga Main CFD Forum 5 March 22, 2005 21:06


All times are GMT -4. The time now is 12:14.