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

ERROR when using rhoSimpleFoam in Helyx-OS

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

Like Tree6Likes
  • 3 Post By spitchers
  • 1 Post By student666
  • 1 Post By bigorange
  • 1 Post By Junyan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 23, 2016, 05:52
Default ERROR when using rhoSimpleFoam in Helyx-OS
  #1
New Member
 
Suffolk
Join Date: Nov 2015
Posts: 26
Rep Power: 10
spitchers is on a distinguished road
Hello guys,

I am currently trying to solve the flow fields for a rotating fan. I have achieved a fully converged solution using the incompressible solver SimpleFoam + MRF.

I then tried to switch to the compressible solver rhoSimpleFoam. I then received the following error:

Code:
******************
*    Run Case    *
******************
Case         : /home/shaun/Engys/HELYX-OS/v2.4.0/Fan-whole
Procs        : 10
Log          : /home/shaun/Engys/HELYX-OS/v2.4.0/Fan-whole/log/rhoSimpleFoam.log
Env          : /home/shaun/OpenFOAM/OpenFOAM-4.1/etc/bashrc
Vendor       : /home/shaun/OpenFOAM
Paraview     : 
MachineFile  : 
Solver       : rhoSimpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.1
Exec   : rhoSimpleFoam -parallel -case /home/shaun/Engys/HELYX-OS/v2.4.0/Fan-whole
Date   : Dec 23 2016
Time   : 10:39:25
Host   : "shaun-VirtualBox"
PID    : 23400
Case   : /home/shaun/Engys/HELYX-OS/v2.4.0/Fan-whole
nProcs : 10
Slaves : 
9
(
"shaun-VirtualBox.23401"
"shaun-VirtualBox.23402"
"shaun-VirtualBox.23403"
"shaun-VirtualBox.23404"
"shaun-VirtualBox.23405"
"shaun-VirtualBox.23406"
"shaun-VirtualBox.23407"
"shaun-VirtualBox.23408"
"shaun-VirtualBox.23409"
)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: convergence criteria
    field U	 tolerance 1e-05
    field k	 tolerance 1e-05
    field epsilon	 tolerance 1e-05
    field omega	 tolerance 1e-05
    field nuTilda	 tolerance 1e-05
    field T	 tolerance 1e-05
    field p_rgh	 tolerance 1e-05
    field p	 tolerance 1e-05

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

AMI: Creating addressing and weights between 10160 source faces and 11916 target faces
AMI: Patch source sum(weights) min/max/average = 0.9935779661, 1.000019777, 0.9999713889
AMI: Patch target sum(weights) min/max/average = 0.9065191601, 1.000053569, 0.9998211027
AMI: Creating addressing and weights between 10160 source faces and 11040 target faces
AMI: Patch source sum(weights) min/max/average = 0.9535948576, 1.000123476, 0.9999134227
AMI: Patch target sum(weights) min/max/average = 0.9320583719, 1.000040807, 0.9997696866
AMI: Creating addressing and weights between 9396 source faces and 36264 target faces
AMI: Patch source sum(weights) min/max/average = 0.9848569855, 1.000234112, 0.99997651
AMI: Patch target sum(weights) min/max/average = 0.9639753469, 1.000449394, 0.9999899062
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    label           "k-\u03C9 SST";
    fieldMaps
    {
        k               k;
        omega           omega;
        nut             nut;
        alphat          alphatCompressible;
    }
    alphaK1         0.85034;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.85616;
    gamma1          0.5532;
    gamma2          0.4403;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    c1              10;
    Cmu             0.09;
    alphah          1.111;
    b1              1;
    F3              false;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: MRF_mrf
Creating finite volume options from "system/fvOptions"


Starting time loop

Time = 1

--> FOAM Warning : 
    From function Foam::fv::gaussConvectionScheme<Type>::gaussConvectionScheme(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>]
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 124
    Reading "/home/shaun/Engys/HELYX-OS/v2.4.0/Fan-whole/system/fvSchemes.divSchemes.div(phi,U)" at line 43
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'warnUnboundedGauss' in "/home/shaun/OpenFOAM/OpenFOAM-4.1/etc/controlDict"
[0] 
[0] 
[0] --> FOAM FATAL ERROR: 
[0] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[0] 
[0]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[0]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[0] 
FOAM parallel run aborting
[0] 
[0] #0  Foam::error::printStack(Foam::Ostream&)[1] 
[1] 
[1] --> FOAM FATAL ERROR: 
[1] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[1] 
[1]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[1]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[1] 
FOAM parallel run aborting
[1] 
[8] 
[8] 
[1] #0  [8] Foam::error::printStack(Foam::Ostream&)--> FOAM FATAL ERROR: 
[8] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[8] 
[8]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[8]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[8] 
FOAM parallel run aborting
[8] 
[8] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[1] #1  Foam::error::abort()[9] 
[9] 
[9] --> FOAM FATAL ERROR: 
[9] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[9] 
[9]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[9]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[9] 
FOAM parallel run aborting
[9] 
 at ??:?
[8] #1  Foam::error::abort()[9] #0  Foam::error::printStack(Foam::Ostream&)[3] 
[3] 
[3] --> FOAM FATAL ERROR: 
[3] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[3] 
[3]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[3]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[3] 
FOAM parallel run aborting
[3] 
[3] #0  Foam::error::printStack(Foam::Ostream&)[2] 
[2] 
[2] --> FOAM FATAL ERROR: 
[2] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[2] 
[2]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[2]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[2] 
FOAM parallel run aborting
[2] 
[6] 
[6] 
[6] --> FOAM FATAL ERROR: 
[6] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[6] 
[6]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[6]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[6] 
FOAM parallel run aborting
[6] 
[2] #0  Foam::error::printStack(Foam::Ostream&)[6] #0  Foam::error::printStack(Foam::Ostream&)[7] 
[7] 
[7] --> FOAM FATAL ERROR: 
[7] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[7] 
[7]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[7]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[7] 
FOAM parallel run aborting
[7] 
[7] #0  Foam::error::printStack(Foam::Ostream&)[5] 
[5] 
[5] --> FOAM FATAL ERROR: 
[5] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[5] 
[5]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[5]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[5] 
FOAM parallel run aborting
[5] 
[5] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[4] 
[4] 
[4] --> FOAM FATAL ERROR: 
[4] 
    [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
[4] 
[4]     From function void Foam::checkMethod(const Foam::fvMatrix<Type>&, const Foam::DimensionedField<Type, Foam::volMesh>&, const char*) [with Type = Foam::Vector<double>]
[4]     in file /home/shaun/OpenFOAM/OpenFOAM-4.1/src/finiteVolume/lnInclude/fvMatrix.C at line 1292.
[4] 
FOAM parallel run aborting
[4] 
[0] #1  Foam::error::abort()[4] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[8] #2   at ??:?
[9] #1  Foam::error::abort() at ??:?
[1] #2   at ??:?
[3] #1  Foam::error::abort() at ??:?
 at ??:?
[7] #1  Foam::error::abort()[2] #1  Foam::error::abort()void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
[0] #2  void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
[6] #1  Foam::error::abort() at ??:?
 at ??:?
[4] #1  Foam::error::abort()[5] #1  Foam::error::abort() at ??:?
[9] #2   at ??:?
[3] #2   at ??:?
[8] #3  void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
[2] #2  void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
[7] #2  void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) at ??:?
[6] #2  ? at ??:?
[5] #2   at ??:?
[1] #3   at ??:?
[9] #3   at ??:?
[0] #3  void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*)void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*)?void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*)void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*)? at ??:?
[4] #2   at ??:?
[8] #4   at ??:?
[3] #3  ? at ??:?
[1] #4   at ??:?
[9] #4   at ??:?
[6] #3   at ??:?
[7] #3  ?void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam::DimensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*)? at ??:?
[2] #3   at ??:?
[5] #3   at ??:?
[0] #4   at ??:?
[4] #3  ? at ??:?
[8] #5  __libc_start_main at ??:?
[3] #4  ????? at ??:?
[1] #5  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[8] #6  ??? at ??:?
[0] #5  __libc_start_main at ??:?
[6] #4   in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #6   at ??:?
[9] #5  __libc_start_main at ??:?
[7] #4  ? at ??:?
[5] #4   at ??:?
[2] #4   in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #6   at ??:?
[3] #5  __libc_start_main? at ??:?
[4] #4  ? at ??:?
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 8 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.
--------------------------------------------------------------------------
? in "/lib/x86_64-linux-gnu/libc.so.6"
[9] #6  ??? at ??:?
[6] #5  __libc_start_main at ??:?
 in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #6  ?? at ??:?
[5] #5  __libc_start_main at ??:?
[7] #5  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[7] #6  ? at ??:?
 in "/lib/x86_64-linux-gnu/libc.so.6"
[6] #6  ? at ??:?
? at ??:?
 at ??:?
 at ??:?
[2] #5  __libc_start_main at ??:?
[4] #5  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[4] #6  ? in "/lib/x86_64-linux-gnu/libc.so.6"
[5] #6  ? at ??:?
[shaun-VirtualBox:23397] 5 more processes have sent help message help-mpi-api.txt / mpi-abort
[shaun-VirtualBox:23397] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
I have read the error and it seems to be that there is a mismatch in the momentum equation terms.

Code:
  [U[0 1 -2 0 0 0 0] ] + [(rho*MRFZoneList:acceleration)[1 -2 -2 0 0 0 0] ]
Has anyone experienced this before? I am running OpenFOAM 4.1 and use Helyx-OS as a GUI for snappyHexMesh and setting up cases.
spitchers is offline   Reply With Quote

Old   April 19, 2017, 03:57
Default
  #2
New Member
 
Michelangelo
Join Date: Apr 2015
Posts: 17
Rep Power: 11
MIZOR is on a distinguished road
Hi spitchers,

I have the same problem. Have you found the solution?
MIZOR is offline   Reply With Quote

Old   April 19, 2017, 05:23
Default
  #3
New Member
 
Suffolk
Join Date: Nov 2015
Posts: 26
Rep Power: 10
spitchers is on a distinguished road
Hi MIZOR,

I did solve the problem. I think I deleted all processor files (for parallel case). Then deleted all files in the 0 time folder (boundary conditions). I then clicked save in Helyx and it re-wrote all the boundary files. From then I Decomposed the file and run the solver.

The problem I was getting was the units in the p file were not correct. I had used the incompressible units and you have to change them for the compressible case.

I hope this helps.


Sent from my iPhone using CFD Online Forum mobile app
vs1, Cagatayemre and Hamzeh193 like this.
spitchers is offline   Reply With Quote

Old   May 14, 2017, 20:16
Default
  #4
Member
 
Di Cheng
Join Date: May 2010
Location: Beijing, China
Posts: 47
Rep Power: 16
chengdi is on a distinguished road
I also encountered this problem this morning and did not resolve it yet. I think I have set the correct IC and BC unit:
------------------------------------------------------------
di@di-VirtualBox:~/OpenFOAM/di-4.1/run/naca0012_7_rhoSimpleFoam$ grep dimensions 0/*
0/alphat:dimensions [1 -1 -1 0 0 0 0];
0/nut:dimensions [0 2 -1 0 0 0 0];
0/nuTilda:dimensions [0 2 -1 0 0 0 0];
0/p://dimensions [0 2 -2 0 0 0 0];
0/p:dimensions [1 -1 -2 0 0 0 0];
0/T:dimensions [0 0 0 1 0 0 0];
------------------------------------------------------------------

I also tried to use incompressible pressure unit. It causes another problem.
chengdi is offline   Reply With Quote

Old   May 17, 2017, 16:49
Default
  #5
Senior Member
 
M. C.
Join Date: May 2013
Location: Italy
Posts: 286
Blog Entries: 6
Rep Power: 17
student666 is on a distinguished road
Hi,

I encountered the same problem; indeed the solution is to set the unit for p file properly.

I'm using simpleFoam with MRF inside; no heat transfer, so it is:

For incompressible p(calculated in foam) = p/rho --> [0 2 -2 0 0 0 0 0]

Regards
vs1 likes this.
student666 is offline   Reply With Quote

Old   December 29, 2021, 13:11
Smile Solution to dimension-check error related to MRF
  #6
New Member
 
Big Orange
Join Date: Mar 2016
Posts: 11
Rep Power: 10
bigorange is on a distinguished road
I have encountered the same problem when I add forceCoefficient functionObject in system/controlDict file. (My case is a 2D case, Z axis is the empty axis, my solver is rhoSimpleFoam)

But when I delete the phi field in 0 directory, the error disappears.
aadicfd likes this.

Last edited by bigorange; December 29, 2021 at 17:51.
bigorange is offline   Reply With Quote

Old   January 20, 2022, 21:45
Default FOAM FATAL ERROR: (openfoam-2012) [h[1 -1 -3 0 0 0 0] ] + [Sc[1 -1 3 0 0 0 0] ]
  #7
New Member
 
ZhuangLi
Join Date: Jan 2022
Posts: 13
Rep Power: 4
zhuangli is on a distinguished road
Quote:
Originally Posted by bigorange View Post
I have encountered the same problem when I add forceCoefficient functionObject in system/controlDict file. (My case is a 2D case, Z axis is the empty axis, my solver is rhoSimpleFoam)

But when I delete the phi field in 0 directory, the error disappears.

Hi! foamer,

The issue you have solved,and do you know why it happened?
anything will be appreciate!


zhuangli
zhuangli is offline   Reply With Quote

Old   March 29, 2022, 10:56
Default
  #8
New Member
 
Join Date: Nov 2016
Posts: 1
Rep Power: 0
Junyan is on a distinguished road
Quote:
Originally Posted by zhuangli View Post
Hi! foamer,

The issue you have solved,and do you know why it happened?
anything will be appreciate!


zhuangli
Hi zhuangli,


I have encountered the same problem today. The solution from Big Orange inspired me and I solved it successfully.



In my case I used potentialFoam before buoyantSimpleFoam, which was actually wrong because potentialFoam is only for incompressible flow. After the potentialFoam, the phi is calculated WITHOUT rho and then be used in buoyantSimpleFoam, leading to a dimension problem, because in buoyantSimpleFoam rho is considered. My solution is just to remove the potentialFoam.



Junyan
aadicfd likes this.
Junyan is offline   Reply With Quote

Reply

Tags
mrfzones, openfoam 4.1, rhosimplefoam error

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
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 8 July 1, 2022 06:54
How to add and select solver in Helyx han0459 OpenFOAM Running, Solving & CFD 1 April 18, 2017 14:46
Huge discrepancy between rhoSimpleFoam and sonicFoam using same boundary conditions!! andreachr OpenFOAM Running, Solving & CFD 0 August 22, 2016 12:26
rhoSimpleFoam angledDuctExplicitFixedCoeff tutorial fails in parallel donQi OpenFOAM Running, Solving & CFD 1 February 22, 2016 19:47
rhoSimpleFoam. patchField error. 123 OpenFOAM Running, Solving & CFD 4 June 6, 2014 15:22


All times are GMT -4. The time now is 02:51.