RunTime Functions: combining "fieldMinMax" and "surface"

Djub · December 14, 2012, 04:16

Hi dear community,

I want to extract from a large unsteady calculation some data, but focusing only on a part of my domain.
So I use the "surfaces" function in my controldict:

Code:

functions {
p_Maison    {
        type surfaces;
        functionObjectLibs ("libsampling.so");
        enabled         true;
        outputControl   timeStep;
        interpolationScheme cellPoint;
        surfaceFormat vtk;
        fields        (      p        );
        surfaces        (
            P_bati            {
                type            patch;
                patches         ( batiment_patch0 );
                interpolate     true;
                triangulate     false;
            }
        );
    }
}

First quesiton: I am quite surprised, because my case works fine, but the official website http://www.openfoam.com/features/run...processing.php does not mention this type ! Is this the same as sampledPatch ?

I want also to isolate the extreme values of this field. I know a bit about the fieldMinMax function.

Second question: I tried from the $FOAM_TUTORIAL folder the Linux command:

Code:

grep -r 'fieldMinMax'

But with no succes (when " grep -r 'fieldAverage' " works...) ! Where to find help about the fieldMinMax function ? More specirfically, what are the necessary entries in the subdictionary ?

Third question: how to combine these two functions ? More precisely, I want to have the min and max values of a given field (here, P) but only on one patch of my calculation. Is it possible to do this?

Thanks a lot for your help

Djub

gschaider · December 23, 2012, 19:38

Quote:

Originally Posted by Djub

Hi dear community,

I want to extract from a large unsteady calculation some data, but focusing only on a part of my domain.
So I use the "surfaces" function in my controldict:

Code:

functions {
p_Maison    {
        type surfaces;
        functionObjectLibs ("libsampling.so");
        enabled         true;
        outputControl   timeStep;
        interpolationScheme cellPoint;
        surfaceFormat vtk;
        fields        (      p        );
        surfaces        (
            P_bati            {
                type            patch;
                patches         ( batiment_patch0 );
                interpolate     true;
                triangulate     false;
            }
        );
    }
}

First quesiton: I am quite surprised, because my case works fine, but the official website http://www.openfoam.com/features/run...processing.php does not mention this type ! Is this the same as sampledPatch ?

I want also to isolate the extreme values of this field. I know a bit about the fieldMinMax function.

Second question: I tried from the $FOAM_TUTORIAL folder the Linux command:

Code:

grep -r 'fieldMinMax'

But with no succes (when " grep -r 'fieldAverage' " works...) ! Where to find help about the fieldMinMax function ? More specirfically, what are the necessary entries in the subdictionary ?

Third question: how to combine these two functions ? More precisely, I want to have the min and max values of a given field (here, P) but only on one patch of my calculation. Is it possible to do this?

Thanks a lot for your help

Djub

@third question: there is always this annoying little voice here on the message board that says "swak4Foam may be the answer". That's be me ... the voice

@second question: one good strategy to find out which parameters are required is to not give any. Then one after one give them to OF until it stops complaining

Djub · January 21, 2013, 05:26

Hi!
I was mistaken with the fieldMinMax function: it gives the extreme value of one field. But I didnot want these values: I am looking for a field of min/max values in time. Saying, for a transient analysis, I would like the two fields Fm dans FM that gives:

for all space point (x,y,z), for all time t, Fm(x,y,z) < F(x,y,z,t) < FM(x,y,z)

These fields represent, for each location, the extreme values in time.

For the moment, I can do this by writing each time step on the hard drive, and then, read them (with MatLab) and calculate the extreme values. But this solution is quite heavy and "expensive" in terms of space disk. I thought it could be possible to calculate these two fields "inline", keeping only the currents field and the two extreme fields.

Any ideas?

gschaider · January 21, 2013, 08:49

Quote:

Originally Posted by Djub

Hi!
I was mistaken with the fieldMinMax function: it gives the extreme value of one field. But I didnot want these values: I am looking for a field of min/max values in time. Saying, for a transient analysis, I would like the two fields Fm dans FM that gives:

for all space point (x,y,z), for all time t, Fm(x,y,z) < F(x,y,z,t) < FM(x,y,z)

These fields represent, for each location, the extreme values in time.

For the moment, I can do this by writing each time step on the hard drive, and then, read them (with MatLab) and calculate the extreme values. But this solution is quite heavy and "expensive" in terms of space disk. I thought it could be possible to calculate these two fields "inline", keeping only the currents field and the two extreme fields.

Any ideas?

Yep ... swak4Foam. The expressionField together with the stored-variables feature. Add this function object:

Code:

calcMin {
   type expressionField;
   fieldName FMin;
   outputControl timeStep;
   outputInterval 1;
   expression "storedMin";
   autowrite true;
   variables (
       "storedMin=min(storedMin,F);"
   );
   storedVariables(
     {
       name storedMin;
       initialValue "1e20";
     }
   );
}

This writes a Field FMin. The value is calculated from the minimum until now. Declaring storedMin as a stored variable makes sure that the value until now is not forgotten (the min-expression wouldn't evaluate without that anyway).

Djub · January 21, 2013, 09:54

Hi Bernhard ,
thanks

for quick reply. I added the libraries in my controldict, and I put your instructions within my functions { ... } . My controlDict looks like:

Code:

...
libs (       
      "libOpenFOAM.so"
      "libsimpleSwakFunctionObjects.so"
      "libswakFunctionObjects.so"
      "libgroovyBC.so"
    );
 
functions
{
    calcMin {
        type     expressionField;
        fieldName    FMin;
        outputControl   timeStep;
        outputInterval    1;
        expression     "storedMin";
        autowrite true;
        variables (    "storedMin=min(storedMin,F);"   );
        storedVariables(
           { name storedMin;
            initialValue "1e20";     
           }    // line 77
        ); 
    }
 
    speed {
        type probes; 
...

But Foam crashes. First a warning:

PHP Code:


			
From function entry::getKeyword(keyType&, Istream&)
    in file db/dictionary/entry/entryIO.C at line 77
    Reading /home/julien/OpenFOAM/julien-2.1.x/run/Mur/processor0/../system/controlDict
    found on line 78 the punctuation token ')'
    expected either } or EOF

and then an error:

PHP Code:


			
[7] --> FOAM FATAL ERROR: 
[7] Unknown function type expressionField
Table of functionObjects is empty

Sorry for this mistake: I think it is a stupid typing error, but I don't see it! What did I make wrong?

gschaider · January 21, 2013, 11:23

Quote:

Originally Posted by Djub

Hi Bernhard ,
thanks

for quick reply. I added the libraries in my controldict, and I put your instructions within my functions { ... } . My controlDict looks like:

Code:

...
libs (       
      "libOpenFOAM.so"
      "libsimpleSwakFunctionObjects.so"
      "libswakFunctionObjects.so"
      "libgroovyBC.so"
    );
 
functions
{
    calcMin {
        type     expressionField;
        fieldName    FMin;
        outputControl   timeStep;
        outputInterval    1;
        expression     "storedMin";
        autowrite true;
        variables (    "storedMin=min(storedMin,F);"   );
        storedVariables(
           { name storedMin;
            initialValue "1e20";     
           }    // line 77
        ); 
    }
 
    speed {
        type probes; 
...

But Foam crashes. First a warning:

PHP Code:


			
From function entry::getKeyword(keyType&, Istream&)

    in file db/dictionary/entry/entryIO.C at line 77

    Reading /home/julien/OpenFOAM/julien-2.1.x/run/Mur/processor0/../system/controlDict

    found on line 78 the punctuation token ')'

    expected either } or EOF

and then an error:

PHP Code:


			
[7] --> FOAM FATAL ERROR: 

[7] Unknown function type expressionField

Table of functionObjects is empty

Sorry for this mistake: I think it is a stupid typing error, but I don't see it! What did I make wrong?

I should have added the disclaimer "typed this from the top of my memory. There may be typos". There should have been a space between "storedVariables" and "(". For OF "(" can be a valid component of a name (contrary what we're used to from C++) that's why the parser is confused when he encounters a ")" (because he "swa" no single "(")

Djub · January 21, 2013, 12:33

It is OK now for the warning, but the error is still there...

OH No! I realize I changed my computer! So I do not have installed swak4foam.

And again I have errors while compiling... (cf http://www.cfd-online.com/Forums/openfoam/103279-contrib-swak4foam.html#post367473)

I am working with GeekoCFD (http://susestudio.com/a/2qtLK2/geekocfd) and I thought sawk4Foam was allready installed...

Tomorrow I will try to fallow my own installation explainations...

Djub · February 11, 2013, 11:31

Hi Bernard,

1/ Finally, the use of swak4foam was very easy and quite straitforward. I did not had to modify nothing; it worked well on his own.

2/ Wonderfull! I can see my fields pmin and pmax changing in time. I suppose now I can use the sample utility on those two fields to restrict the field on focus the attention only in my patch.

Thanks a lot! I knew that swak4foam was awesome , know I know it will save me hours of coding!

Simple, efficient, clear: bravo to swak4foam!

cfd@kgp · December 11, 2016, 09:37

Dear All,

I have tried to create a new field using both---1. coded functions and
2. using expressionField as given below,

I am applying this quoted text to the standard tutorial of "hotRoom" in buoyantPimpleFoam

Quote:

functions
{
compute_ptot
{
functionObjectLibs ( "libutilityFunctionObjects.so" );
type coded;
// enabled true;
redirectType ptot;
outputControl outputTime;
// outputInterval 1;
code
#{

const volVectorField& U = mesh().lookupObject<volVectorField>("U");
volScalarField mymagu
(
IOobject
(
"mymagu",
mesh().time().timeName(),
U.mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mag(U)
);
mymagu.write();

#};
}

compute_ptot
{
type expressionField;
outputControl outputTime;
outputInterval 1;
fieldName ptot;
expression "(mag(U))";
autowrite true;
}
};

with following libraries

Quote:

libs (

"libsimpleSwakFunctionObjects.so"

"libswakFunctionObjects.so"

);

In both the method I can see the output files of the variables "mymagu" and "compute_ptot", but they are not readable in paraview.

I found out that when we run the application with " -withFunctionObjects " paraFoam know the new field written when I tried the same quoted text to the standard tutorial of "cylinder" in potentialFoam, I can isualize the new field in paraFoam.

But " -withFunctionObjects " fails with buoyantPimpleFoam

Quote:

buoyantPimpleFoam -withFunctionObjects

produces following error,

Quote:

Usage: buoyantPimpleFoam [OPTIONS]
options:
-case <dir> specify alternate case directory, default is the cwd
-noFunctionObjects
do not execute functionObjects
-parallel run in parallel
-roots <(dir1 .. dirN)>
slave root directories for distributed running
-srcDoc display source code in browser
-doc display application documentation in browser
-help print the usage

Using: OpenFOAM-3.0.1 (see www.OpenFOAM.org)
Build: 3.0.1-18e358711b4e

--> FOAM FATAL ERROR:
Invalid option: -withFunctionObjects

FOAM exiting

Is this a bug in openfoam or I am making some mistake?

Please help

Thanks and regards.

Esmaeelef · September 10, 2017, 19:32

Quote:

Originally Posted by gschaider

I should have added the disclaimer "typed this from the top of my memory. There may be typos". There should have been a space between "storedVariables" and "(". For OF "(" can be a valid component of a name (contrary what we're used to from C++) that's why the parser is confused when he encounters a ")" (because he "swa" no single "(")

Hi Bernhard,

I am trying to use functionObject libraries in swak4foam to calculate some fields. I have successfully installed Openfoam 222 and the compatible version of swak4foam (https://github.com/Unofficial-Extend...-swak4Foam.git swak4Foam) on an HPC cluster. The problem is that I receive the following error while using swak4foam
"
Unknown function type expressionField

Valid functions are :

9
(
initSwakFunctionObject
partialWrite
patchProbes
probes
removeRegisteredObject
sets
surfaces
writeDictionary
writeRegisteredObject
)
"
Looking at the libraries compiled by Swak4FOAM, I found that FunctionObject is not in the list of compiled libraries, though Swak4FOAM has been correctly installed. Here is the list of compiled libraries:

libgroovyBC.so
libgroovyStandardBCs.so
libsimpleLagrangianFunctionObjects.so
libsimpleSearchableSurfaces.so
libswak4FoamParsers.so
libswakChemistryModelFunctionPlugin.so
libswakCoalCloudAdaptor.so
libswakDynamicMeshFunctionPlugin.so
libswakDynamicMesh.so
libswakFvcSchemesFunctionPlugin.so
libswakFvOptions.so
libswakLagrangianCloudSourcesFunctionPlugin.so
libswakLagrangianParser.so
libswakLocalCalculationsFunctionPlugin.so
libswakMeshQualityFunctionPlugin.so
libswakMeshWaveFunctionPlugin.so
libswakMRFFunctionPlugin.so
libswakQuantileFunctionPlugin.so
libswakRandomFunctionPlugin.so
libswakSourceFields.so
libswakSurfacesAndSetsFunctionPlugin.so
libswakThermoTurbFunctionPlugin.so
libswakTopoSources.so
libswakTransportTurbFunctionPlugin.so

Is there any specific reason why FunctionObject does not exist in the list of libraries?

Thank you in advance for your time and support.
Kind Regards
Esmaeel

gschaider · September 11, 2017, 17:01

Quote:

Originally Posted by Esmaeelef

Hi Bernhard,

I am trying to use functionObject libraries in swak4foam to calculate some fields. I have successfully installed Openfoam 222 and the compatible version of swak4foam (https://github.com/Unofficial-Extend...-swak4Foam.git swak4Foam) on an HPC cluster. The problem is that I receive the following error while using swak4foam
"
Unknown function type expressionField

Valid functions are :

9
(
initSwakFunctionObject
partialWrite
patchProbes
probes
removeRegisteredObject
sets
surfaces
writeDictionary
writeRegisteredObject
)
"
Looking at the libraries compiled by Swak4FOAM, I found that FunctionObject is not in the list of compiled libraries, though Swak4FOAM has been correctly installed. Here is the list of compiled libraries:

libgroovyBC.so
libgroovyStandardBCs.so
libsimpleLagrangianFunctionObjects.so
libsimpleSearchableSurfaces.so
libswak4FoamParsers.so
libswakChemistryModelFunctionPlugin.so
libswakCoalCloudAdaptor.so
libswakDynamicMeshFunctionPlugin.so
libswakDynamicMesh.so
libswakFvcSchemesFunctionPlugin.so
libswakFvOptions.so
libswakLagrangianCloudSourcesFunctionPlugin.so
libswakLagrangianParser.so
libswakLocalCalculationsFunctionPlugin.so
libswakMeshQualityFunctionPlugin.so
libswakMeshWaveFunctionPlugin.so
libswakMRFFunctionPlugin.so
libswakQuantileFunctionPlugin.so
libswakRandomFunctionPlugin.so
libswakSourceFields.so
libswakSurfacesAndSetsFunctionPlugin.so
libswakThermoTurbFunctionPlugin.so
libswakTopoSources.so
libswakTransportTurbFunctionPlugin.so

Is there any specific reason why FunctionObject does not exist in the list of libraries?

Thank you in advance for your time and support.
Kind Regards
Esmaeel

Have you added libswakFunctionObjects.so to the libs-list in controlDict? (BTW: I don't see that library in your list)

Esmaeelef · September 11, 2017, 18:12

Quote:

Originally Posted by gschaider

Have you added libswakFunctionObjects.so to the libs-list in controlDict? (BTW: I don't see that library in your list)

Hi Bernhard,

Thanks for your response. Yes, I have added libswakFunctionObject.so to the controlDict:

libs ( "libIOFunctionObjects.so" "libOpenFOAM.so" "libgroovyBC.so" "libswakFunctionObjects.so");

Below is the list of libraries compiled after compiling swak4foam, I do not know why libswakFunctionObject is not in the list, while swak4foam was successfully compiled. Is there any way to add libswakFunctionObject to other compiled swak4foam libraries?

libgroovyBC.so
libgroovyStandardBCs.so
libsimpleLagrangianFunctionObjects.so
libsimpleSearchableSurfaces.so
libswak4FoamParsers.so
libswakChemistryModelFunctionPlugin.so
libswakCoalCloudAdaptor.so
libswakDynamicMeshFunctionPlugin.so
libswakDynamicMesh.so
libswakFvcSchemesFunctionPlugin.so
libswakFvOptions.so
libswakLagrangianCloudSourcesFunctionPlugin.so
libswakLagrangianParser.so
libswakLocalCalculationsFunctionPlugin.so
libswakMeshQualityFunctionPlugin.so
libswakMeshWaveFunctionPlugin.so
libswakMRFFunctionPlugin.so
libswakQuantileFunctionPlugin.so
libswakRandomFunctionPlugin.so
libswakSourceFields.so
libswakSurfacesAndSetsFunctionPlugin.so
libswakThermoTurbFunctionPlugin.so
libswakTopoSources.so
libswakTransportTurbFunctionPlugin.so

gschaider · September 12, 2017, 07:15

Quote:

Originally Posted by Esmaeelef

Hi Bernhard,

Thanks for your response. Yes, I have added libswakFunctionObject.so to the controlDict:

libs ( "libIOFunctionObjects.so" "libOpenFOAM.so" "libgroovyBC.so" "libswakFunctionObjects.so");

Below is the list of libraries compiled after compiling swak4foam, I do not know why libswakFunctionObject is not in the list, while swak4foam was successfully compiled. Is there any way to add libswakFunctionObject to other compiled swak4foam libraries?

libgroovyBC.so
libgroovyStandardBCs.so
libsimpleLagrangianFunctionObjects.so
libsimpleSearchableSurfaces.so
libswak4FoamParsers.so
libswakChemistryModelFunctionPlugin.so
libswakCoalCloudAdaptor.so
libswakDynamicMeshFunctionPlugin.so
libswakDynamicMesh.so
libswakFvcSchemesFunctionPlugin.so
libswakFvOptions.so
libswakLagrangianCloudSourcesFunctionPlugin.so
libswakLagrangianParser.so
libswakLocalCalculationsFunctionPlugin.so
libswakMeshQualityFunctionPlugin.so
libswakMeshWaveFunctionPlugin.so
libswakMRFFunctionPlugin.so
libswakQuantileFunctionPlugin.so
libswakRandomFunctionPlugin.so
libswakSourceFields.so
libswakSurfacesAndSetsFunctionPlugin.so
libswakThermoTurbFunctionPlugin.so
libswakTopoSources.so
libswakTransportTurbFunctionPlugin.so

There seems to be a problem with the compilation. Essential libraries like libsimpleFunctionObjects.so and libswakFunctionObjects.so are missing. Rerun Allwmake and check the output

December 14, 2012, 04:16	RunTime Functions: combining "fieldMinMax" and "surface"	#1
Djub Senior Member Julien Join Date: Jun 2012 Location: France Posts: 152 Rep Power: 13	Hi dear community, I want to extract from a large unsteady calculation some data, but focusing only on a part of my domain. So I use the "surfaces" function in my controldict: Code: functions { p_Maison { type surfaces; functionObjectLibs ("libsampling.so"); enabled true; outputControl timeStep; interpolationScheme cellPoint; surfaceFormat vtk; fields ( p ); surfaces ( P_bati { type patch; patches ( batiment_patch0 ); interpolate true; triangulate false; } ); } } First quesiton: I am quite surprised, because my case works fine, but the official website http://www.openfoam.com/features/run...processing.php does not mention this type ! Is this the same as sampledPatch ? I want also to isolate the extreme values of this field. I know a bit about the fieldMinMax function. Second question: I tried from the $FOAM_TUTORIAL folder the Linux command: Code: grep -r 'fieldMinMax' But with no succes (when " grep -r 'fieldAverage' " works...) ! Where to find help about the fieldMinMax function ? More specirfically, what are the necessary entries in the subdictionary ? Third question: how to combine these two functions ? More precisely, I want to have the min and max values of a given field (here, P) but only on one patch of my calculation. Is it possible to do this? Thanks a lot for your help Djub mm.abdollahzadeh likes this.

January 21, 2013, 09:54		#5
Djub Senior Member Julien Join Date: Jun 2012 Location: France Posts: 152 Rep Power: 13	Hi Bernhard , thanks for quick reply. I added the libraries in my controldict, and I put your instructions within my functions { ... } . My controlDict looks like: Code: ... libs ( "libOpenFOAM.so" "libsimpleSwakFunctionObjects.so" "libswakFunctionObjects.so" "libgroovyBC.so" ); functions { calcMin { type expressionField; fieldName FMin; outputControl timeStep; outputInterval 1; expression "storedMin"; autowrite true; variables ( "storedMin=min(storedMin,F);" ); storedVariables( { name storedMin; initialValue "1e20"; } // line 77 ); } speed { type probes; ... But Foam crashes. First a warning: PHP Code: `From function entry::getKeyword(keyType&, Istream&) in file db/dictionary/entry/entryIO.C at line 77 Reading /home/julien/OpenFOAM/julien-2.1.x/run/Mur/processor0/../system/controlDict found on line 78 the punctuation token ')' expected either } or EOF` and then an error: PHP Code: `[7] --> FOAM FATAL ERROR: [7] Unknown function type expressionField Table of functionObjects is empty` Sorry for this mistake: I think it is a stupid typing error, but I don't see it! What did I make wrong?

January 21, 2013, 05:26		#3
Djub Senior Member Julien Join Date: Jun 2012 Location: France Posts: 152 Rep Power: 13	Hi! I was mistaken with the fieldMinMax function: it gives the extreme value of one field. But I didnot want these values: I am looking for a field of min/max values in time. Saying, for a transient analysis, I would like the two fields Fm dans FM that gives: for all space point (x,y,z), for all time t, Fm(x,y,z) < F(x,y,z,t) < FM(x,y,z) These fields represent, for each location, the extreme values in time. For the moment, I can do this by writing each time step on the hard drive, and then, read them (with MatLab) and calculate the extreme values. But this solution is quite heavy and "expensive" in terms of space disk. I thought it could be possible to calculate these two fields "inline", keeping only the currents field and the two extreme fields. Any ideas?

January 21, 2013, 12:33		#7
Djub Senior Member Julien Join Date: Jun 2012 Location: France Posts: 152 Rep Power: 13	It is OK now for the warning, but the error is still there... OH No! I realize I changed my computer! So I do not have installed swak4foam. And again I have errors while compiling... (cf http://www.cfd-online.com/Forums/openfoam/103279-contrib-swak4foam.html#post367473) I am working with GeekoCFD (http://susestudio.com/a/2qtLK2/geekocfd) and I thought sawk4Foam was allready installed... Tomorrow I will try to fallow my own installation explainations...

February 11, 2013, 11:31		#8
Djub Senior Member Julien Join Date: Jun 2012 Location: France Posts: 152 Rep Power: 13	Hi Bernard, 1/ Finally, the use of swak4foam was very easy and quite straitforward. I did not had to modify nothing; it worked well on his own. 2/ Wonderfull! I can see my fields pmin and pmax changing in time. I suppose now I can use the sample utility on those two fields to restrict the field on focus the attention only in my patch. Thanks a lot! I knew that swak4foam was awesome , know I know it will save me hours of coding! Simple, efficient, clear: bravo to swak4foam!