CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > OpenFOAM

Error in LRR (RAS) model in OpenFOAM v4.1

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

LinkBack Thread Tools Search this Thread Display Modes
Old   February 8, 2017, 18:32
Default Error in LRR (RAS) model in OpenFOAM v4.1
New Member
Inquisitor101's Avatar
Join Date: Jan 2017
Posts: 2
Rep Power: 0
Inquisitor101 is on a distinguished road
I was trying some simple tutorial about a backward-facing step in steady state via different turbulence models in RAS using the simpleFoam solver. One of which was the LRR (Reynolds stress model). The tutorials themselves were done so in another version of OpenFOAM and the one I am using was the latest version: 4.1.

All else worked splendidly, however in the case of the LRR, I keep getting an error returned from the fvSchemes file. Basically, the steps in this method that I am following are: after copying the kEpsilon file (by file I mean the whole kEpsilon simulation folder -- i.e. the directory containing: 0/ constant/ system/ ), I execute the command:

simpleFoam -postProcess -func R
I get, instead of the expected R file, a file named turbulenceProperties:R in the 0/ directory. Moving on, I rename it to R.

Next, I change the turbulence model from kEpsilon to LRR as intended. Afterwards, I edit the fvSchemes and include the following for the divergence terms:

    default             none;
    div(phi,U)         bounded Gauss linearUpwind grad(U);
    div(phi,k)          bounded Gauss linearUpwind grad(k);
    div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon);
    div(phi,omega)  bounded Gauss limitedLinear 1;
    div(phi,v2)        bounded Gauss limitedLinear 1;
    div(phi,R)         bounded Gauss upwind;
    div(R)              Gauss linear;
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
    div(nonlinearStress)             Gauss linear;
Then, after running the command simpleFoam, I get the following error:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

SIMPLE: convergence criteria
    field p     tolerance 0.01
    field U     tolerance 0.001
    field "(k|epsilon|omega|f|v2|R)"     tolerance 0.001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model LRR

cannot find file

file: /home/username/OpenFOAM/username-4.1/run/tutorials/incompressible/simpleFoam/bfs/BFS_baseCase/0/R at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 72.

FOAM exiting
Then, after trying different stuff, I came up with the following and it worked. I simply change the default condition (in the divSchemes) from a none into some other scheme (e.g. Gauss linear) and all worked splendid.

My question hence is why did this happen? is there anything wrong with my implementation or is it a bug ?

Thanks !
Inquisitor101 is offline   Reply With Quote

Old   July 29, 2018, 22:28
Senior Member
Ruiyan Chen
Join Date: Jul 2016
Location: Hangzhou, China
Posts: 157
Rep Power: 6
cryabroad is on a distinguished road
Take a look at this thread


According to Dr. Jasak, "It does not recognise it because this is a straightforward div(thing) term and not convection div(phi, thing). Therefore you cannot do upwinding, since there's no flux to decide the direction from."
cryabroad is offline   Reply With Quote

Old   July 2, 2020, 15:09
New Member
Giacomo Del Bianco
Join Date: Jul 2020
Location: Venice area - Italy
Posts: 2
Rep Power: 0
Giacomodb is on a distinguished road
Thank you very much!! You fixed my problem.

I saw browsing from the internet but I didn't realized it was different from the one:

div((nuEff*dev2(T(grad(U))))) Gauss linear;
Later I got another error:

keyword wallDist is undefined in dictionary
I googled it and i added at the end of fvSolutions the following definition:

    method meshWave;
Then it worked fine!

Thank you very much again!!

Giacomodb is offline   Reply With Quote


fvschemes, openfoam4.0, ras

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Simulating an aether model of EM using OpenFoam? lamare Electromagnetics 2 September 15, 2016 05:08
Prandtl's one-equation RAS turbulence model Djub OpenFOAM Running, Solving & CFD 3 April 9, 2016 06:30
about Subgrid-scale model impecca OpenFOAM Running, Solving & CFD 4 December 20, 2013 10:36
OpenFOAM: LES turbulence model names Ollie OpenFOAM 5 January 7, 2013 10:24
Water subcooled boiling Attesz CFX 7 January 5, 2013 03:32

All times are GMT -4. The time now is 18:13.