CFD Online Discussion Forums - pressureTools postProcessing function objects in 2.2.0

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

- OpenFOAM Post-Processing (https://www.cfd-online.com/Forums/openfoam-post-processing/)

- - pressureTools postProcessing function objects in 2.2.0 (https://www.cfd-online.com/Forums/openfoam-post-processing/118267-pressuretools-postprocessing-function-objects-2-2-0-a.html)

Greetings to all!

@Brock: That wasn't possible in OpenFOAM 2.2, but it is possible to do in OpenFOAM 2.3. The source code file in question is this:

Code:

$FOAM_SRC/postProcessing/functionObjects/utilities/pressureTools/pressureTools.C

As of 2.3.0, at the end of each time step, it will execute the calculation of this requested pressure.

Best regards,
Bruno

Hi!

Thank you GRAUPS, it works perfectly now!

Now I hop this static pressure field can be used to change from simpleFoam to rhoSimpleFoam :)

Best regards
Benjamin

Quote:

Originally Posted by wyldckat (Post 506268)

As of 2.3.0, at the end of each time step, it will execute the calculation of this requested pressure.

@Bruno: Thanks for your comment. You are correct, OpenFOAM 2.3 now executes the calculation after every time-step.

Quote:

Originally Posted by BenJ (Post 506835)

Thank you GRAUPS, it works perfectly now!

@Ben: Glad I could help!

Dear all,

I'm trying to get "pressureTools" function to work with simpleFoam but I get the error shown below. I've checked and the files were definitely compiled so should be available to call. Can anyone offer an insight?

Thanks,

James :D

Code:

--> FOAM FATAL ERROR: 

Unknown function type pressureTools



Valid functions are : 



17

(

cellSource

faceSource

fieldAverage

fieldCoordinateSystemTransform

fieldMinMax

fieldValueDelta

nearWallFields

patchProbes

probes

processorField

readFields

regionSizeDistribution

sets

streamLine

surfaceInterpolateFields

surfaces

wallBoundedStreamLine

)

My function call looks like this:

Code:

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

| =========                 |                                                 |

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

|  \\    /   O peration     | Version:  2.2.1                                 |

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

|    \\/     M anipulation  |                                                 |

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



 pressuretools1   // user-defined name of function object entry

    {

        type            pressureTools;

        libs ("libutilityFunctionObjects.so");

        //region          defaultRegion;

        enabled         yes;

        //timeStart       0;

        //timeEnd         10;

        outputControl timeStep;//outputTime;//

        outputInterval 1; // 5000;

        calcTotal   yes;

        calcCoeff   yes;

    }





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

So.. I have had some success!

I need to change the library reference to:
functionObjectLibs ("libutilityFunctionObjects.so");

However, I then needed to specify:
pRef
pInf
rhoInf
UInf

And the result was total pressure coefficient (Cp0) being calculated but not static pressure coefficient (Cp)? Will the function only calculate one or the other or can you get it to calculate both?

The modes of operation are:
\table
Mode | calcTotal | calcCoeff
static pressure | no | no
total pressure | yes | no
pressure coefficient | no | yes
total pressure coefficient | yes | yes
\endtable

Any advice gratefully received!
Thanks

Greetings James,

Sorry for the very late reply, but only today did I finally manage to take a look into this.
From what I can see from another post you've done, you've found a solution:

Quote:

Originally Posted by jrwrodgers (Post 513198)

I'm by no means an expert but when through a similar exercise a week ago. I found that to calculate the coefficients both static and total you need to specify the reference static pressure and reference velocity within the pressureTools {}. OF didn't pick up the values from the boundary conditions. I think I ended up specifying also the reference density although this is superfluous for the incompressible simulation I was running.

In addition to your finding, the answer to your previous post:

Quote:

Originally Posted by jrwrodgers (Post 511441)

And the result was total pressure coefficient (Cp0) being calculated but not static pressure coefficient (Cp)? Will the function only calculate one or the other or can you get it to calculate both?

... is that you would need to add two function object entries instead of just one, e.g.:

Code:

pressuretools1

{

//...

}



pressuretools2

{

//...

}

Only then will your be able to get the two types of results calculations.

Best regards,
Bruno

Is it possible to write an areaAverage pressure along an axis as asked here using pressure tools?
Thanks

Quote:

Originally Posted by canopus (Post 577903)

Is it possible to write an areaAverage pressure along an axis as asked here using pressure tools?

Quick (late) answer: "pressureTools" currently only calculates for the whole pressure field. You could then use one of the resulting fields to be averaged instead of the "p" field.

Hi there,

Is it possible to use pressureTools as a sample instead of functionObject? I added this piece of code to my controlDict:

Code:

functions

   {

       pressureTools1

       {

                type         pressureTools;

                functionObjectLibs ("libutilityFunctionObjects.so");

                source                wall;

                sourceName        cylinder;

                

                log                yes; 

                

                outputControl        timeStep;

                outputInterval        1; 

                

                //enabled        yes; 

                calcTotal        no;

                calcCoeff        yes;

                pRef                0;

                rhoInf                1.0;

                pInf                101325;

                UInf                (0.4208 0 0);                

       }

       



   }

Which did something really weird on running... data was written to more time steps and the velocity field was not saved except at the written time steps, so I couldn't properly postprocess anything (or view the simulation in paraview or paraFoam).

Two questions:
1) Can I set this up in my sampleDict instead?
2) I really just want to calculate the total pressure at probes on the cylinder to calculate the drag from that.... is this the best way to do it?

Quick answers:

Quote:

Originally Posted by arieljeds (Post 594108)

Code:

outputControl    timeStep;

outputInterval    1;

Try changing to this:

Code:

outputControl outputTime;

For more details:

Code documentation: http://foam.sourceforge.net/docs/cpp/index.html
- "Post-processing" near the bottom of the page will take you here: http://foam.sourceforge.net/docs/cpp/a00004.html
  - Several details about function objects on that page.

Quote:

Originally Posted by arieljeds (Post 594108)

1) Can I set this up in my sampleDict instead?

After the function object has done its job, either while the solver was running or by running execFlowFunctionObjects, these pressure fields will have been written to the time folder(s).
Then you can use sample to sample over the data in the written fields.

Quote:

Originally Posted by arieljeds (Post 594108)

2) I really just want to calculate the total pressure at probes on the cylinder to calculate the drag from that.... is this the best way to do it?

Another alternative I can think of is the tutorial "incompressible/simpleFoam/motorBike/", which in file "system/forceCoeffs" has an example of a function object for calculating the Cd and Cl, if I remember correctly. This file is included by the file "system/controlDict", which is why it will be executed while the solver is running.

Hi wyldckat,

Thank you for your very thorough response... I have two follow up questions/issues now:

1) I am trying to run execFlowFunctionObjects, which is giving the error that the keyword transport properties is undefined..However, here is my transportProperties file:

Code:

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

| =========                 |                                                 |

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

|  \\    /   O peration     | Version:  2.1.0                                 |

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

|    \\/     M anipulation  |                                                 |

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

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    location    "constant";

    object      transportProperties;

}

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



phases (water air);



water

{

    transportModel  Newtonian;

    nu              nu [ 0 2 -1 0 0 0 0 ] 0.0631;        // Re = 40

    rho             rho [ 1 -3 0 0 0 0 0 ] 1028;

    

    CrossPowerLawCoeffs

    {

        nu0             nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;

        nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;

        m               m [ 0 0 1 0 0 0 0 ] 1;

        n               n [ 0 0 0 0 0 0 0 ] 0;

    }



    BirdCarreauCoeffs

    {

        nu0             nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;

        nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;

        k               k [ 0 0 1 0 0 0 0 ] 99.6;

        n               n [ 0 0 0 0 0 0 0 ] 0.1003;

    }

    

}



air

{

    transportModel  Newtonian;

    nu              nu [ 0 2 -1 0 0 0 0 ] 1.568e-05; //1.48e-05;  --> current measurement for kinematic viscosity found at engineeringtoolbox.com

    rho             rho [ 1 -3 0 0 0 0 0 ] 1;

    

    CrossPowerLawCoeffs

    {

        nu0             nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;

        nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;

        m               m [ 0 0 1 0 0 0 0 ] 1;

        n               n [ 0 0 0 0 0 0 0 ] 0;

    }



    BirdCarreauCoeffs

    {

        nu0             nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;

        nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;

        k               k [ 0 0 1 0 0 0 0 ] 99.6;

        n               n [ 0 0 0 0 0 0 0 ] 0.1003;

    }

    

}



sigma           sigma [ 1 0 -2 0 0 0 0 ] 0.07;





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

In this, because the transportModel is Newtonian, I have assumed that the CrossPowerLaw and BirdCarreau stuff is ignored. Is this correct?

2) I am trying to really understand what the pressure I am getting is because I was having issues implementing the calculating for dragForce, and so I want to calculate it from the pressures instead so I can better understand it. In waveFoam, I am calculating two pressures: p_rgh and p. I am understanding that p_rgh is a reference pressure that is calculated and p would then be p = p_rgh + rho*g*h, which would mean then that the total pressure, and then pressures used in the calculation for pressure coefficient, Cp, would be: p + 0.5*rho*Uinf^2 (where I've been taking Uinf from a probe near the inlet). I'll say now that doing it this way has not been yielding results for the Cp that I'm expecting (as in, the value that I'm calculating for Cp is far too high). Is there something I am misunderstanding about the pressures?

Thanks again for your help,
Ariel

Quote:

Originally Posted by wyldckat (Post 434184)

Hi Ehsan,

Took me a while to get to here, but here goes:

You told me through an email that if you used swak4Foam, you only needed 1 function instead of 3.
Guess what!? swak4Foam 0.2.4 is already available, at least through SVN and at my GitHub account https://github.com/wyldckat/swak4foam (look for the big ZIP button).
(Side note: Bernhard was at the OFW8 these past days and I think he hasn't had the time to do the final announcements, but he has already provided these news over Twitter.
... edit: never mind, he's on top of things :): http://www.cfd-online.com/Forums/ope...tml#post433484 post #29)
With this version of swak4Foam, which builds without problems with OpenFOAM 2.2.0, the following additional code for the function object should work as expected:

Code:

outputControlMode outputTime; outputInterval 1;

__________________

As for the original issue on the previous post, I'll quote what I've already sent you through emails - The following function objects worked well together:

Code:

functions

{

    writeMissingFields

    {

        type writeRegisteredObject;

        functionObjectLibs ( "libIOFunctionObjects.so" );

        objectNames ("phi");

        outputControl     outputTime;

    }

//................................................................................

    totalP    // user-defined name of function object entry

    {

        type            pressureTools;

        libs            ("libutilityFunctionObjects.so");

        //region          defaultRegion;

        enabled         yes;

        //timeStart       0;

        //timeEnd         10;

        outputControl timeStep;//outputTime;//

        outputInterval 1; // 5000;

        calcTotal   yes;

        calcCoeff   no;

        pRef 0;

    }





    Average_left

    {

        type           faceSource;

        functionObjectLibs ("libfieldFunctionObjects.so");

        enabled on;

        log             yes;

        valueOutput     false;

        surfaceFormat   vtk;

        source          patch;

        sourceName      left;

        operation       areaAverage;

        fields

        (

            p

            //phi // surface fields not supported for sampledSurface

            T

            rho

            h

            U

        );

        outputControl timeStep;//outputTime;//

        outputInterval 1; // 5000;

      }

      reloadTotalP

      {

          type        readFields;

          functionObjectLibs ("libfieldFunctionObjects.so");

          //region          defaultRegion;

          enabled         yes;

          //timeStart       0;

          //timeEnd         10;

          outputControl timeStep;//outputTime;//

          outputInterval 1; // 5000;

          fields

          (

              "total(p)"

          );

      }

      totalPressure_left

      {

        $Average_left;

        operation       weightedAverage;

        weightField     rho;

        

        fields

        (

          total(p)

        );

      }

}

Notes:

The function object "readFields" was needed for reloading back into memory the field "total(p)".
As for time folders that only have the field "total(p)": it's because of how the function object was created. It only calculates when it has to write the field to file and it is not registered into memory, which is why we have to use "readFields" for loading it back.
For this function object to always calculate the field and save it only occasionally, this would require to edit the original source code for the "pressureTools" function object.

Best regards,
Bruno

Hi,

Can anyone help with the running of this code through chtMultiRegionFoam? (I am using OpenFOAM 6)

I have copied the above into my controlDict folder and I have tried running the following:

chtMultiRegionFoam -postProcess -func writeMissingFields

chtMultiRegionFoam -postProcess -func totalP
chtMultiRegionFoam -postProcess -func Average_left
chtMultiRegionFoam -postProcess -func reloadTotalP

chtMultiRegionFoam -postProcess -func totalPressure_left

in that order.

-I've also tried it without the inclusion of chtMultiRegionFoam in the above order.
-I've also tried running each part seperately as well, but it still doesn't work - I don't get a postProcessing folder, or any sort of results.

I have changed the patch name to the one I require - cyclicFluidInlet. I am completely at a loss, if anyone could help then I would be very greatful.

I have included my controlDict as well (I had to zip it to upload), any other information can be supplied.

Thanks,
Arthur

Quick answer: I see that you later on have gotten an answer to your question here: https://www.cfd-online.com/Forums/op...egionfoam.html

Essentially there were two issues:

"-region regionName" was a missing argument in the command, where "regionName" is the name of the region you wanted to process.
"-func" is not meant to be used with each individual entry inside the controlDict. You could execute without the "-func name" and it would run all of those function objects that were indicated in the controlDict.

Quote:

Originally Posted by wyldckat (Post 719910)

Quick answer: I see that you later on have gotten an answer to your question here: https://www.cfd-online.com/Forums/op...egionfoam.html

Essentially there were two issues:

"-region regionName" was a missing argument in the command, where "regionName" is the name of the region you wanted to process.
"-func" is not meant to be used with each individual entry inside the controlDict. You could execute without the "-func name" and it would run all of those function objects that were indicated in the controlDict.

Yeah, it was a general mix up of about 4 different solutions combined which wasn't the best way to go about it. I ended up taking the function object out of the control dict and just made a script to run post processing with the required functions (- func <function>) within that instead which worked a treat!