[chamoun]

I would like to post-process OpenFoam velocity field data with Matlab. For this, I am going to use the 'points' file located in constant>polyMesh>points. I am also going to use a 'U' file. The points file containts more rows than the U file. I'm assuming this is the case because the points file contains the boundary points, while the U file does not. This presents a problem

Does anyone know what the correspondence is between these two data files? I need to know which points have which velocities, and which points are on the boundary, and which are in the interior of the boundary?

thanks!

[ngj]

The points in OpenFoam are the the corners of any computational cell, e.g. a hex-cell is made out of 8 points. The velocity is computed in the cell centres of these computational cells, hence there should not be a direct correspondence.

Use the tool "writeCellCentres" to achieve the cell centres, which corresponds to those in the velocity file.

Best regards,

Niels

[chamoun]

Thanks for the help. I looked up writeCellCentres.C in the documentation, but they don't have an example of how to enter it into the solver. Is this straightforward or more involved? Any help would be appreciated!

thank you

[ngj]

You cannot make it a part of the solver, as it is a stand-alone postprocessing tool. Just type writeCellCentres in the command line when you have completed the computation, and the cell centres will be written to each time directory.

Type "writeCellCentres -help" if you are unsure how to use it.

Best regards,

Niels

[chamoun]

Tak, Niels!

[jeicek]

Hello Guys,

I typed writeCellCenters and it creates files in each time step with names of 'ccx ,ccy and ccz' but the strange thing is that the dimension of these ccx ccy ccz are only m or in other words their dimension is length and not the velocity also their values are not corresponding with U file!!!??? am I wrong?? do you have any idea?

[alexeym]

Hi,

Units for coordinates of the centers of cells should be in meters. Why would they be in meters per second?

[jeicek]

Hi Alexeym, then what are these 'ccx ,ccy and ccz' ?? Aren't they the velocity components in x,y and z directions in the cell center?!?!? if not then what are they?

[jeicek]

Originally Posted by alexeym

Hi,

Units for coordinates of the centers of cells should be in meters. Why would they be in meters per second?

Hi Alexeym,then what are these 'ccx ,ccy and ccz' ?? Aren't they the velocity components in x,y and z directions in the cell center?!?!? if not then what are they?

[alexeym]

Hi,

no, they are not. Reread the name of the utility - write cell centers. Look at the code of utility:

        for (direction i=0; i<vector::nComponents; i++)
        {
            volScalarField cci
            (
                IOobject
                (
                    "cc" + word(vector::componentNames[i]),
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh.C().component(i)
            );

            cci.write();
        }

mesh.C() is an array of cell centers (i.e. coordinates of cell centers).

If you'd like to get velocity components use foamCalc.

[jeicek]

Thank you very much Alexym for clarifying, now it was cleared for me.

[Elham]

Hi,

I want to know the coordinates of cell centres coresponding to Ug values. Ug is gradient of U that is created by calcFvcGrad. I have used writeCellCentres to have ccx, ccy and ccz. But the number of data that I have for them is a bit more than the number of data that I have for Ug; 515618 for coordinates and 503367 for gradient.

Anyone can help me to find the right coordinate for UGrad?

Thanks

[pattim]

Hi Neils - I tried typing writeCellCentres at the linux command line (after sourcing the bashrc file for OF) and it doesn't exist. On a search, I found a directory named writeCellCentres in the subdir /usr/lib/openfoam/openfoam2112/src/functionObjects/field/ containing two files - a header and a C file. Do we have to rebuild all the utilities in that subdir before they can be used?


Please help! Thanks!

(base) patti@linux-lhkc:/OSS/Data_drive/users/00__OF_Combustion_2021-2023/n-Butane_100> setfoam 
bash@OpenFoam >>> writeCellCentres -help 
If 'writeCellCentres' is not a typo you can use command-not-found to lookup the package that contains it, like this: 
    cnf writeCellCentres 
bash@OpenFoam >>> ./writeCellCentres -help 
bash: ./writeCellCentres: No such file or directory 
bash@OpenFoam >>> 

Originally Posted by ngj

You cannot make it a part of the solver, as it is a stand-alone postprocessing tool. Just type writeCellCentres in the command line when you have completed the computation, and the cell centres will be written to each time directory.

Type "writeCellCentres -help" if you are unsure how to use it.

Best regards,

Niels

[Krapf]

In the current versions of OpenFOAM it is no longer a stand-alone application, but a function object: OpenFOAM 10, OpenFOAM v2112.

[pattim]

Thank you very much for the reply, Krapf. I thought it might be a version difference. So now I'm not sure how to use writeCellCentres in my runs. (I guess I only need it to run once)

Do I put this code example, for instance, in controDict or some other OF run file? BTW: the API guide for v2112

Usage
    Minimal example by using system/controlDict.functions:

    writeCellCentres
    {
        // Mandatory entries (unmodifiable)
        type        writeCellCentres;
        libs        (fieldFunctionObjects);

        // Optional (inherited) entries
        ...
    }

The API guide for v2112 also lists...

Minimal example by using the postProcess utility:
postProcess -func writeCellCentres

This runs with some OF screen output - but I didn't see any outputs... Hmmm,maybe I need to "reconstruct" the (parallel) case first... (runApplication -append reconstructPar)

Originally Posted by Krapf

In the current versions of OpenFOAM it is no longer a stand-alone application, but a function object: OpenFOAM 10, OpenFOAM v2112.

[pattim]

Thank you very much - I was able to create files, but I'm not sure how to read them. They are, like the raw datafiles, mixtures of ASCII and what appears to be (compressed?) binary data. Is there a utility to convert the data to ASCII for easy reading? (I don't see such an option in postProcess -func writeCellCentres -help-full) I was able to export the written cell center data to ASCII (as ".csv" files) using paraFoam - but I was just wondering if there was a specific OF command I'm not finding.


Thanks,
PattiM

Edit: I was able to load the output of writeCellCenters into paraFoam and to write them to CSV files from paraFoam - the but number of points output by paraFoam is 12,283 points, whereas my 2D solution is on 48x126 = 6,048cells. This may arise because I'm exporting from paraFoam. Isn't there a way to output a flat acsii data file directly from OpenFoam that can be to imported into matlab/python/etc.? Anyone?


Edit2: The final fix was to use the python package "openfoamparser" - no issues with formats, etc.