CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Post-Processing

Age of Air Function Object

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

Like Tree1Likes
  • 1 Post By b.simpson

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 1, 2020, 11:54
Default Age of Air Function Object
  #1
New Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 18
Rep Power: 3
b.simpson is on a distinguished road
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);
					}
				}
			}
		}
	}
I am now getting the following error:
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
Does anyone know what I need to put in place of "injectionRateSuSp"?

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"
}
fvSolutions:
Code:
AoA
    {
        solver           smoothSolver;
        smoother         GaussSeidel;
        tolerance        1e-08;
        relTol           0.1;
        nsweep           1;
    }
fvSchemes:
Code:
div(phi,AoA) bounded Gauss upwind;
b.simpson is offline   Reply With Quote

Old   December 7, 2020, 17:46
Default
  #2
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 116
Rep Power: 4
Tobermory is on a distinguished road
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);
					}
				}
to something like:

Code:
				sources
				{
					AoA
					{
						explicit 1;
						implicit 0;
					}
				}
Good luck!
Tobermory is offline   Reply With Quote

Old   December 10, 2020, 09:27
Default Thanks
  #3
New Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 18
Rep Power: 3
b.simpson is on a distinguished road
Thank you for your reply Tobermory.

The changes you suggested worked and my AoA is now working.

Many thanks.

Ben
Tobermory likes this.
b.simpson is offline   Reply With Quote

Reply

Tags
age of air, buoyantsimplefoam, natural ventilation, openfoam 8

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
[Other] refineWallLayer Error Yuby OpenFOAM Meshing & Mesh Conversion 1 May 19, 2017 11:13
[OpenFOAM] Annoying issue of automatic "Rescale to Data Range " with paraFoam/paraview 3.12 keepfit ParaView 60 September 18, 2013 04:23
Compile problem ivanyao OpenFOAM Running, Solving & CFD 1 October 12, 2012 10:31
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51
[blockMesh] Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Meshing & Mesh Conversion 10 April 2, 2007 15:00


All times are GMT -4. The time now is 15:05.