|
[Sponsors] |
December 1, 2020, 10:54 |
Age of Air Function Object
|
#1 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6 |
Hi all,
I am trying to set up an Age of Air function object in OpenFOAM 8. I am running buoyantSimpleFoam in Ubuntu 18.04. I have tried implementing a function object from older threads (mainly Age of air with function object). My controlDict code is: Code:
AoA { type scalarTransport; libs ("libutilityFunctionObjects.so"); enabled true; writeControl writeTime; log yes; nCorr 1; field AoA; active true; autoSchemes false; resetOnStartUp false; DT 1e-5; fvOptions { IncrementTime { type semiImplicitSource; active true; selectionMode all; volumeMode specific; sources { injectionRateSuSp { AoA (1 0); } } } } } Code:
Selecting finite volume options model type semiImplicitSource Source: IncrementTime - selecting all cells - selected 1119784 cell(s) with volume 158.70844 [0] [0] [0] --> FOAM FATAL ERROR: [0] request for regIOobject injectionRateSuSp from objectRegistry region0 failed available objects of type regIOobject are Or if there is a better method for calculating age of air? Thanks in advance for any support. Kind regards, Ben My 0/AoA file is: Code:
FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object AoA; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 1 0 0 0 0]; internalField uniform 0; boundaryField { "xmin|xmax|ymin|ymax|zmax_north|zmax_south" { type fixedValue; value uniform 0; } "zmin|Ceiling|Floor|East_Wall|North_Wall|South_Wall|West_Wall|Computer|Person|zmax_ceiling" { type zeroGradient; } Inlet { type fixedValue; value uniform 0; } #includeEtc "caseDicts/setConstraintTypes" } Code:
AoA { solver smoothSolver; smoother GaussSeidel; tolerance 1e-08; relTol 0.1; nsweep 1; } Code:
div(phi,AoA) bounded Gauss upwind; |
|
December 7, 2020, 16:46 |
|
#2 |
Senior Member
Join Date: Apr 2020
Location: UK
Posts: 668
Rep Power: 14 |
There were some changes in v8 to the semiImplicit source term syntax. Check out https://openfoam.org/release/8/ and the example in https://github.com/OpenFOAM/OpenFOAM...7e9747fe696aeb. I am guessing that you need to change:
Code:
sources { injectionRateSuSp { AoA (1 0); } } Code:
sources { AoA { explicit 1; implicit 0; } } |
|
December 10, 2020, 08:27 |
Thanks
|
#3 |
Member
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6 |
Thank you for your reply Tobermory.
The changes you suggested worked and my AoA is now working. Many thanks. Ben |
|
February 7, 2021, 13:40 |
|
#4 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 932
Rep Power: 12 |
In case of anyone's interest,
Function object definitions for the `local mean age of air` and `normalised local mean age of air` metrics (where zero-value means fresh air): Code:
scalarTransport1 { type scalarTransport; libs (solverFunctionObjects); field LMA; schemesField k; // bounded Gauss limitedLinear 1; bounded01 false; alphaD 1; // viscous contribution alphaDt 0; // turbulent contribution // Adding fvOption source for residence time fvOptions { unitySource { type scalarSemiImplicitSource; enabled true; scalarSemiImplicitSourceCoeffs { selectionMode all; volumeMode specific; injectionRateSuSp { LMA (1 0); } } } } resetOnStartUp false; timeStart <timeStart>; executeControl timeStep; executeInterval 1; writeControl writeTime; } normalisedLocalMeanAge1 { type reference; libs (fieldFunctionObjects); field LMA; result nLMA; // normT = T / (V/Q) // normT: normalised local mean age of air // T: local mean age of air (Bartak et al., 2001, Eq. 1) // V: volume of air in the room [m3] // Q: volumetric flow rate through the inlet [m3/s] // V/Q: (estimated) mean age of fluid through a reference area (e.g. outlet) // scale = 1/(V/Q) = Q/V [1/s] scale <Q/V>; offset 0; timeStart <timeStart>; executeControl writeTime; writeControl writeTime; } Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2012 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object LMA; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0; boundaryField { inlet { type fixedValue; value uniform 0; } outlet { type inletOutlet; inletValue uniform 0; value uniform 0; } ".*" { type zeroGradient; } #includeEtc "caseDicts/setConstraintTypes" } // ************************************************************************* // Code:
solvers { LMA { solver PBiCGStab; preconditioner DILU; tolerance 1e-8; relTol 0.01; } } relaxationFactors { equations { LMA 0.7; } }
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
August 13, 2021, 01:38 |
|
#5 |
New Member
Toby
Join Date: Aug 2021
Posts: 1
Rep Power: 0 |
@HPE:
Thanks for providing the code for the function object, I successfully implemented it into my case. However, analysing the results uncovered some unrealistic values where the LMA value was bigger than the timestep (e.g. after 40 s the LMA showed a value of 60). Any idea where this mistake might originate from? I am simulating a box-shaped room with natural ventilation (inlet and outlet window). Thanks in advance! |
|
Tags |
age of air, buoyantsimplefoam, natural ventilation, openfoam 8 |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Other] refineWallLayer Error | Yuby | OpenFOAM Meshing & Mesh Conversion | 2 | November 11, 2021 11:04 |
[OpenFOAM] Annoying issue of automatic "Rescale to Data Range " with paraFoam/paraview 3.12 | keepfit | ParaView | 60 | September 18, 2013 03:23 |
Compile problem | ivanyao | OpenFOAM Running, Solving & CFD | 1 | October 12, 2012 09:31 |
Problem with rhoSimpleFoam | matteo_gautero | OpenFOAM Running, Solving & CFD | 0 | February 28, 2008 06:51 |
[blockMesh] Axisymmetrical mesh | Rasmus Gjesing (Gjesing) | OpenFOAM Meshing & Mesh Conversion | 10 | April 2, 2007 14:00 |