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

rhoSimpleFoam unknown RASModel type laminar

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 6, 2016, 10:40
Default rhoSimpleFoam unknown RASModel type laminar
  #1
New Member
 
Thomas A
Join Date: Mar 2016
Posts: 6
Rep Power: 2
tdog is on a distinguished road
Hello
I'm trying to do a compressible simulation using rhoSimpleFoam for a laminar flow. The scripts I am using is based on an earlier OpenFOAM version (2.0 I think) as was working there, but I am running the newest version.

When I run my scripts I get the following error:
"--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
"
Where my turbulenceProperties is set to the following:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  RAS;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //
As far as I can tell from the documentation (http://cfd.direct/openfoam/user-guide/turbulence/) I am doing it the right wa, what seems to be the problem?
tdog is offline   Reply With Quote

Old   June 7, 2016, 16:40
Default
  #2
New Member
 
Thomas A
Join Date: Mar 2016
Posts: 6
Rep Power: 2
tdog is on a distinguished road
Has nobody tried something similar?
tdog is offline   Reply With Quote

Old   June 8, 2016, 09:38
Default
  #3
Member
 
VA
Join Date: Mar 2015
Location: IN, USA
Posts: 30
Rep Power: 3
vabishek is on a distinguished road
Quote:
Originally Posted by tdog View Post
Hello
I'm trying to do a compressible simulation using rhoSimpleFoam for a laminar flow. The scripts I am using is based on an earlier OpenFOAM version (2.0 I think) as was working there, but I am running the newest version.

When I run my scripts I get the following error:
"--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
"
Where my turbulenceProperties is set to the following:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  RAS;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //
As far as I can tell from the documentation (http://cfd.direct/openfoam/user-guide/turbulence/) I am doing it the right wa, what seems to be the problem?
Not sure if you have fixed it yet but the simulationType should be set to "laminar". If you read the above documentation carefully, it is mentioned at the very beginning.
vabishek is offline   Reply With Quote

Old   June 8, 2016, 10:20
Default
  #4
New Member
 
Thomas A
Join Date: Mar 2016
Posts: 6
Rep Power: 2
tdog is on a distinguished road
@vabishek thank you for your help. I already tried that, but it still produces the same error:
Selecting RAS turbulence model laminar


--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  laminar;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //
tdog is offline   Reply With Quote

Old   June 8, 2016, 10:24
Default
  #5
Member
 
VA
Join Date: Mar 2015
Location: IN, USA
Posts: 30
Rep Power: 3
vabishek is on a distinguished road
Quote:
Originally Posted by tdog View Post
@vabishek thank you for your help. I already tried that, but it still produces the same error:
Selecting RAS turbulence model laminar


--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  laminar;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //
Well, it should look something like this

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType laminar;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}


// ************************************************************************* //
As the error message says, just pick one RASModel from the given list. As you can see, "laminar" is not listed there. If you set simulationType to laminar, it doesn't really mattter what you set RASModel to. Hope that helps!
vabishek is offline   Reply With Quote

Old   June 8, 2016, 10:54
Default
  #6
New Member
 
Thomas A
Join Date: Mar 2016
Posts: 6
Rep Power: 2
tdog is on a distinguished road
Arg, thanks for the tip

Just tried, but still got an error message because I then need to supply files for the boundary conditions - because in theory it shouldn't need them because it's running the simulation as laminar, but those are turbulent models, right?
tdog is offline   Reply With Quote

Old   June 9, 2016, 07:32
Default
  #7
Member
 
Pedro
Join Date: Nov 2014
Posts: 49
Rep Power: 3
pupo is on a distinguished road
This bug seems to have been fixed "recentely"

check the following Commit: https://github.com/OpenFOAM/OpenFOAM...2940548af3ebb3

If your createFields.H in BuyoantSimpleFoam looks like this:

Code:
autoPtr<compressible::RASModel> turbulence
(
     compressible::New<compressible::RASModel>
      (
          rho,
          U,
          phi,
          thermo
     )
 );
change it to:

Code:
autoPtr<compressible::turbulenceModel> turbulence
 (
     compressible::turbulenceModel::New
      (
          rho,
          U,
          phi,
          thermo
     )
 );
cheers
pupo is offline   Reply With Quote

Old   June 11, 2016, 06:31
Default
  #8
New Member
 
Peter F
Join Date: Jun 2016
Posts: 1
Rep Power: 0
peterf is on a distinguished road
I can't locate the applications folder in order to change createFields.H. How do I do this?

I am running OpenFOAM via Docker on a Mac. So I don't really see a path or folder for OpenFOAM. I have tried to show the hidden folders, but the OpenFOAM or applications folder still doesn't appear.
peterf is offline   Reply With Quote

Old   September 9, 2016, 04:58
Default
  #9
Member
 
annn
Join Date: Jun 2016
Posts: 34
Rep Power: 2
cleoo is on a distinguished road
Quote:
Originally Posted by vabishek View Post
Well, it should look something like this

Code:
simulationType laminar;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}
does it actually read the entries in the RAS part if you specified the simulationType as being laminar?

whats the difference between this:
Code:
simulationType RAS;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}
and

Code:
simulationType laminar;
because isn't turbulence off technically just laminar flow?

Last edited by cleoo; September 9, 2016 at 05:00. Reason: fogot sometin
cleoo 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
Divergent with rhoSimpleFoam and the boundary condition problems qjh888 OpenFOAM Running, Solving & CFD 0 May 17, 2016 20:31
time step continuity problem in VAWT simulation lpz_michele OpenFOAM Running, Solving & CFD 4 October 15, 2015 06:19
Boundary Conditions MtnRunBeachBum OpenFOAM Pre-Processing 1 April 30, 2015 16:33
Mesh conversion problem (fluent3DMeshToFoam) Aadhavan OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 December 12, 2012 11:38
compressible two phase flow in CFX4.4 youngan CFX 0 July 1, 2003 23:32


All times are GMT -4. The time now is 22:52.