Post processing an internal plane/surface

CallumG · November 22, 2021, 05:18

Hi Foamers,

I know there are a few threads on this but I am incredibly confused with them all and I know some of the information is outdated so I'm going to ask again.

I'm generating very large case files on our server and I want to postProcess single planes of data for export.

I have a very simple rectangular domain and I would like to "slice/cut plane/internal surface" (whatever you want to call it!) so I am taking the field data from central y-normal and x-normal planes and later view them in ParaView.

Could anyone clarify (for dummies!) how to do this?

I should mention I'm on v1912.

Cheers,
Callum

tomf · November 24, 2021, 05:15

Hi Callum,

There is a tutorial that uses the surfaces functionObject for this.

Please have a look at:

$FOAM_TUTORIALS/incompressible/pimpleFoam/RAS/propeller/

The relevant files are the controlDict and the surfaces files in the system folder. As you see, the surfaces file is read in the functions subDict of the controlDict. The example usage of the surfaces functionObject is described in the surfaces file.

You would need to modify it towards your needs, but I think you should get it from there.

Cheers,
Tom

CallumG · December 14, 2021, 04:22

Hi Tom,

thanks very much for your reply and the advice!

For the benefit of others I ended up adding the following to my controlDict:

Code:

functions
{    
    cuttingPlanes
    {
        type              surfaces;
        outputControl     timeStep;
        outputInterval     1;
        surfaceFormat    vtk;
        fields   (U alpha.water);
        interpolationScheme          cellPoint;
        surfaces
            (
                yplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (0 -5.5 0);
                    normal (0 -1 0);
                }
                interpolate true;
                }
                xplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (5 0 0);
                    normal (1 0 0);
                }
                interpolate true;
                }
            );
    }
}

This made vtk's for each plane I created (xplane and yplane) in my postProcessing directory for each timestep. After that I needed to make a series file to view the vtk's continuosly in Paraview. I did this in python and the code looked something like this:

Code:

import os

def main():
    cutPlanesDir = "postProcessing/cuttingPlanes/"

    directories = os.listdir(cutPlanesDir)
    directories.sort()
    directories = [d for d in directories if "series" not in d]

    with open(cutPlanesDir+"yplane.vtp.series", 'w') as yf:
        yf.write("{\n")
        yf.write("  \"file-series-version\" : \"1.0\",\n")
        yf.write("  \"files\" : [\n")
    with open(cutPlanesDir+"yplane.vtp.series", 'a') as yf:
        for time in directories:
            if time != directories[-1]:
                yf.write("    { \"name\" : \""+time+"/yplane.vtp\", \"time\" : "+time+" },\n")
            else:
                yf.write("    { \"name\" : \""+time+"/yplane.vtp\", \"time\" : "+time+" }\n")
        yf.write("  ]\n")
        yf.write("}")

    with open(cutPlanesDir+"xplane.vtp.series", 'w') as yf:
        yf.write("{\n")
        yf.write("  \"file-series-version\" : \"1.0\",\n")
        yf.write("  \"files\" : [\n")
    with open(cutPlanesDir+"xplane.vtp.series", 'a') as yf:
        for time in directories:
            if time != directories[-1]:
                yf.write("    { \"name\" : \""+time+"/xplane.vtp\", \"time\" : "+time+" },\n")
            else:
                yf.write("    { \"name\" : \""+time+"/xplane.vtp\", \"time\" : "+time+" }\n")
        yf.write("  ]\n")
        yf.write("}")
    return

if __name__ == "__main__":
    main()

Thanks again community, hope this is useful for others!

Callum

tomf · December 14, 2021, 04:29

Hi Callum,

Glad you got it working.

Just a final hint (also for others) as there is a utility in OpenFOAM that can do the 'series' for you. It is called foamSequenceVTKFiles. If you have the .vtp extension it is invoked as:

Code:

foamSequenceVTKFiles -vtp

This will create a folder sequencedVTK with links inside that folder to the original files and the naming is sequential, such that ParaView can interpret this as a series of files. May safe some additional disk space/time.

Cheers,
Tom

CallumG · December 14, 2021, 05:29

Excellent Tom!

I only wrote my own script because when I tried the command foamSequenceVTKFiles it didn't work, which I'm assuming is because I didn't use the flag '-vtp'.

Brilliant! Merry Christmas Foamers!!

olesen · December 16, 2021, 03:49

Quote:

Originally Posted by CallumG

Hi Tom,

thanks very much for your reply and the advice!

For the benefit of others I ended up adding the following to my controlDict:

Code:

functions
{    
    cuttingPlanes
    {
        type              surfaces;
        outputControl     timeStep;
        outputInterval     1;
        surfaceFormat    vtk;
        fields   (U alpha.water);
        interpolationScheme          cellPoint;
        surfaces
            (
                yplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (0 -5.5 0);
                    normal (0 -1 0);
                }
                interpolate true;
                }
                xplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (5 0 0);
                    normal (1 0 0);
                }
                interpolate true;
                }
            );
    }
}

This made vtk's for each plane I created (xplane and yplane) in my postProcessing directory for each timestep. After that I needed to make a series file to view the vtk's continuosly in Paraview.
....

I am a bit surprised at your result. I know that the Ensight and VTK surface writers both add time-collation to their output, but the VTK writers should ideally also be creating the series file. This is either an oversight, or not feasible for some other reason - it could be worthwhile adding an issue on develop.openfoam.com - if nothing else, at least to document why it is that way.

BTW: all of the machinery for generating vtk.series files is already in there (src/fileFormats) and it is most certainly being used for foamToVTK, for example.

farzadmech · September 24, 2023, 14:57

Thanks a lot for your explanation, it was helpful.

Farzad

Quote:

Originally Posted by CallumG

Hi Tom,

thanks very much for your reply and the advice!

For the benefit of others I ended up adding the following to my controlDict:

Code:

functions
{    
    cuttingPlanes
    {
        type              surfaces;
        outputControl     timeStep;
        outputInterval     1;
        surfaceFormat    vtk;
        fields   (U alpha.water);
        interpolationScheme          cellPoint;
        surfaces
            (
                yplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (0 -5.5 0);
                    normal (0 -1 0);
                }
                interpolate true;
                }
                xplane
                {
                type cuttingPlane;
                planeType pointAndNormal;
                pointAndNormalDict
                {
                    point (5 0 0);
                    normal (1 0 0);
                }
                interpolate true;
                }
            );
    }
}

This made vtk's for each plane I created (xplane and yplane) in my postProcessing directory for each timestep. After that I needed to make a series file to view the vtk's continuosly in Paraview. I did this in python and the code looked something like this:

Code:

import os

def main():
    cutPlanesDir = "postProcessing/cuttingPlanes/"

    directories = os.listdir(cutPlanesDir)
    directories.sort()
    directories = [d for d in directories if "series" not in d]

    with open(cutPlanesDir+"yplane.vtp.series", 'w') as yf:
        yf.write("{\n")
        yf.write("  \"file-series-version\" : \"1.0\",\n")
        yf.write("  \"files\" : [\n")
    with open(cutPlanesDir+"yplane.vtp.series", 'a') as yf:
        for time in directories:
            if time != directories[-1]:
                yf.write("    { \"name\" : \""+time+"/yplane.vtp\", \"time\" : "+time+" },\n")
            else:
                yf.write("    { \"name\" : \""+time+"/yplane.vtp\", \"time\" : "+time+" }\n")
        yf.write("  ]\n")
        yf.write("}")

    with open(cutPlanesDir+"xplane.vtp.series", 'w') as yf:
        yf.write("{\n")
        yf.write("  \"file-series-version\" : \"1.0\",\n")
        yf.write("  \"files\" : [\n")
    with open(cutPlanesDir+"xplane.vtp.series", 'a') as yf:
        for time in directories:
            if time != directories[-1]:
                yf.write("    { \"name\" : \""+time+"/xplane.vtp\", \"time\" : "+time+" },\n")
            else:
                yf.write("    { \"name\" : \""+time+"/xplane.vtp\", \"time\" : "+time+" }\n")
        yf.write("  ]\n")
        yf.write("}")
    return

if __name__ == "__main__":
    main()

Thanks again community, hope this is useful for others!

Callum

November 22, 2021, 05:18	Post processing an internal plane/surface	#1
CallumG Member Callum Guy Join Date: Dec 2019 Location: Scotland Posts: 44 Rep Power: 6	Hi Foamers, I know there are a few threads on this but I am incredibly confused with them all and I know some of the information is outdated so I'm going to ask again. I'm generating very large case files on our server and I want to postProcess single planes of data for export. I have a very simple rectangular domain and I would like to "slice/cut plane/internal surface" (whatever you want to call it!) so I am taking the field data from central y-normal and x-normal planes and later view them in ParaView. Could anyone clarify (for dummies!) how to do this? I should mention I'm on v1912. Cheers, Callum

November 24, 2021, 05:15		#2
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 634 Rep Power: 32	Hi Callum, There is a tutorial that uses the surfaces functionObject for this. Please have a look at: $FOAM_TUTORIALS/incompressible/pimpleFoam/RAS/propeller/ The relevant files are the controlDict and the surfaces files in the system folder. As you see, the surfaces file is read in the functions subDict of the controlDict. The example usage of the surfaces functionObject is described in the surfaces file. You would need to modify it towards your needs, but I think you should get it from there. Cheers, Tom Last edited by tomf; November 24, 2021 at 05:16. Reason: grammar

December 14, 2021, 04:29		#4
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 634 Rep Power: 32	Hi Callum, Glad you got it working. Just a final hint (also for others) as there is a utility in OpenFOAM that can do the 'series' for you. It is called foamSequenceVTKFiles. If you have the .vtp extension it is invoked as: Code: foamSequenceVTKFiles -vtp This will create a folder sequencedVTK with links inside that folder to the original files and the naming is sequential, such that ParaView can interpret this as a series of files. May safe some additional disk space/time. Cheers, Tom Teresa Sun likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
wind turbine - post processing	er_ijaz	FLUENT	0	September 30, 2013 05:28
post processing for CEL expressions	Niru	CFX	0	May 10, 2013 13:13
Automated post processing using CFD Post	shreyasr	ANSYS	0	January 28, 2013 06:21
post processing in CFX11.0	u k jha	CFX	1	September 17, 2010 05:53
post processing in CFD	MANISH BHARGAVA	Main CFD Forum	0	October 17, 1998 20:51

December 14, 2021, 05:29		#5
CallumG Member Callum Guy Join Date: Dec 2019 Location: Scotland Posts: 44 Rep Power: 6	Excellent Tom! I only wrote my own script because when I tried the command foamSequenceVTKFiles it didn't work, which I'm assuming is because I didn't use the flag '-vtp'. Brilliant! Merry Christmas Foamers!!