CFD Online Discussion Forums - execFlowFunctionObjects and the noFlow option in v1706

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - execFlowFunctionObjects and the noFlow option in v1706 (https://www.cfd-online.com/Forums/openfoam/190409-execflowfunctionobjects-noflow-option-v1706.html)

execFlowFunctionObjects and the noFlow option in v1706

Hello all,

In the past, we used execFlowFunctionObjects to calculate things like Cp or CpTot after a run had finished, often weeks later when nut, and other unecessary post processing variables had already been deleted for disk space savings. We used the noFlow option, to supress loading nut, and other variables not needed for the task at hand (say calculating Cp.) According to the help, -noFlow "suppress[es] creating flow models" We loved this!

In 1706, execFlowFunctionObjects has been replaced with the postProcess function, which I bloody hate, but that's another story.... postProcess, called either alone or through the solver (simpleFoam -postProcess) doesn't seem to have the -noFlow option that execFlowFunctionObjects had.

Furthermore, execFlowFunctionObjects would execute pressureTools (renamed as "pressure" in 1706, god knows why). With postProcess, I only have access to "totalPressureIncompressible," meaning I cannot call what used to be pressureTools. So it seems I cannot calculate Cp after a case has finished running?

So then, my two questions are:
1.) how can I calculate Cp, and CpTot. I only see totalP possible
2.) how can I do this without nut, like with -noFlow in the past
3.) If anyone knows why execFlowFunctions, which was brilliant, was replaced by postProcess, which seems to be less featured and harder to use?

Hi,

I understand your frustration, as the functionality changed significantly. However you can still do what you want and it is actually simplified when you know how to do it.

Unfortunately there is a lack of documentation in logical places as far as I am concerned, but from the CFD Direct online user guide one can learn about command line interface postprocessing and than some trial and error usually gets me what I want.

For your case you can run:

Code:

postProcess -func "totalPressureIncompressible(p,U)" -latestTime

and have the file totalPressureIncompressible in your system folder with the following entries (modified to your case):

Code:

/*--------------------------------*- C++ -*----------------------------------*\

  =========                 |

  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox

|  \\    /   O peration     | Version:  plus                                  |  

|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

     \\/     M anipulation  |

-------------------------------------------------------------------------------

Description

    Calculates the total pressure field for a case where the solver is

    incompressible (pressure is kinematic, e.g. m^2/s^2).



\*---------------------------------------------------------------------------*/



#includeEtc "caseDicts/postProcessing/pressure/pressure.cfg"



calcTotal     yes;

calcCoeff     yes;

rho           rhoInf;

pInf          0.0;

UInf          (15 0 0);

pRef          0.0;

rhoInf        1.2;



// ************************************************************************* //

Regards,
Tom

Thanks Tom! I think it's less usable than the old way, but so is life....

Question: do you call out U and P ("totalPressureIncompressible(p,U)") in order to suppress reading excess flow variables, as was accomplished in the past with the -noFlow option?

Sorry for the late reply, but was on vacation. I think you specify U and p because those are necessary fields for the computation, but I am not sure. You could try running with and without it and see the difference...

Regards,
Tom