|
[Sponsors] |
OpenFOAM 1.7 cylindricalInletVelocity and swirlFlowRateInletVelocity BC's |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 29, 2010, 11:49 |
OpenFOAM 1.7 cylindricalInletVelocity and swirlFlowRateInletVelocity BC's
|
#1 |
New Member
Adam Comer
Join Date: Jun 2010
Posts: 6
Rep Power: 15 |
I am very new to this software and recently installed OF1.7 beside OF1.6 to use the new boundary conditions.
I am trying to use the new swirl/cylindrical boundary conditions in OF 1.7, but I get the error below even though I follow the format specified in the header files for these bc's. The file should not need a 'value' line according to the header. Also, I have checked that my shell is searching OF1.7 directories for files by running a solver (fireFoam) that does not exist in my non-updated version of OF1.6. Finally, I am trying to do this on a nonplanar mesh that was produced by snappyHexMesh. Thanks in advance for any help. Adam Reading field U --> FOAM FATAL IO ERROR: Essential entry 'value' missing file: /home/alc79/OpenFOAM/OpenFOAM-1.7.0/tutorials/mesh/combustor_jetson_swirl_coldflow_refined/2e-07/U::boundaryField::comb_injector_inlet from line 79 to line 84. From function fvPatchField<Type>::fvPatchField(const fvPatch& p,const DimensionedField<Type, volMesh>& iF,const dictionary& dict,const bool valueRequired) in file /home/alc79/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/fvPatchField.C at line 120. FOAM exiting |
|
June 29, 2010, 12:33 |
|
#2 |
Senior Member
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 23 |
Yes, I was just looking at that, and also changed it to accept a velocity instead of a flowrate. Just include value, it needs that to place the calculated velocities in. It shouldn't matter what you put there.
Code:
inlet { type swirlFlowRateInletVelocity; flowRate 0.2; // Volumetric/mass flow rate [m3/s or kg/s] rpm 100; value uniform (0 0 0); }
__________________
Laurence R. McGlashan :: Website |
|
June 30, 2010, 04:10 |
|
#3 |
New Member
Adam Comer
Join Date: Jun 2010
Posts: 6
Rep Power: 15 |
Thanks a lot. The same value line seems to be needed for the cylindricalInletVelocity BC as well.
Many Thanks. Adam |
|
December 8, 2010, 08:51 |
|
#4 |
New Member
Join Date: Mar 2010
Posts: 25
Rep Power: 16 |
Hi Adam (or someone else),
can you please post your BC with the cylindricalInletVelocity. With best regards |
|
December 8, 2010, 08:56 |
|
#5 |
New Member
Adam Comer
Join Date: Jun 2010
Posts: 6
Rep Power: 15 |
For a patch named AIR_INLET
AIR_INLET { type cylindricalInletVelocity; axis (0 1 0); centre (0 0.114 0); axialVelocity 2.202582536; rpm 444.4074; radialVelocity 0; value uniform (0 0 0); } |
|
December 8, 2010, 11:34 |
|
#6 |
New Member
Join Date: Mar 2010
Posts: 25
Rep Power: 16 |
Looks like my first trial.
Thank you for the fast reply. Now it's running. |
|
February 1, 2017, 04:11 |
|
#7 |
New Member
Pierre
Join Date: Oct 2011
Posts: 15
Rep Power: 14 |
Hi,
With swirlFlowRateInletVelocity, I don't know how to determine if "flowRate" is mass or volume flow rate. According to the code, it depends on units of "phi" Code:
if (phi.dimensions() == dimVelocity*dimArea) { // volumetric flow-rate operator==(tangentialVelocity + n*avgU); } else if (phi.dimensions() == dimDensity*dimVelocity*dimArea) { const fvPatchField<scalar>& rhop = patch().lookupPatchField<volScalarField, scalar>(rhoName_); // mass flow-rate operator==(tangentialVelocity + n*avgU/rhop); } Thanks, Pierre |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Floating object tutorial case in OpenFOAM 1.7 | sega | OpenFOAM Running, Solving & CFD | 11 | February 9, 2012 04:29 |
Installation how-to's - OpenFOAM 1.7 - openSUSE 11.2 and 11.3 | alberto | OpenFOAM Installation | 24 | August 4, 2010 00:48 |
OpenFOAM 1.7 - openSUSE 11.3 - gcc 4.5.0 | alberto | OpenFOAM | 12 | July 28, 2010 11:59 |
Modified OpenFOAM Forum Structure and New Mailing-List | pete | Site News & Announcements | 0 | June 29, 2009 05:56 |
Adventure of fisrst openfoam installation on Ubuntu 710 | jussi | OpenFOAM Installation | 0 | April 24, 2008 14:25 |