Function object for strain rate tensor?

blebon · August 9, 2017, 07:47

Dear Foamers,

Is there a way of outputting the strain rate using function objects?

The strainRate is already calculated in viscosityModel:

Code:

Foam::tmp<Foam::volScalarField> Foam::viscosityModel::strainRate() const
{
    return sqrt(2.0)*mag(symm(fvc::grad(U_)));
}

I would like to output this field from a calculated case with -postProcess.

Thanks

blebon · August 9, 2017, 08:35

Never mind, found a solution and posting it if anyone interested in the future. Just create a new function object to recalculate the strain rate. Copy the vorticity fn object and rename strainRate, change the curl include line to #include "fvcGrad.H" and edit the calc function as follows:

Code:

bool Foam::functionObjects::strainRate::calc()
{
    if (foundObject<volVectorField>(fieldName_))
    {
        return store
        (
            resultName_,
            sqrt(2.0)*mag(symm(fvc::grad(lookupObject<volVectorField>(fieldName_))))
        );
    }
    else
    {
        return false;
    }

    return true;
}

pibil1 · September 1, 2017, 18:38

Hello blebon,

Thanks Can you help me on how to implement this please?, I have copied /opt/openfoam4/src/functionObjects/field/vorticity to /opt/openfoam4/src/functionObjects/field/strainRate. Then replaced everything that says vorticity to strainRate in both strainRate.H and strainRate.C. Then added #include "fvcGrad.H" in strainRate.H and rewrote the calc funcion.

Please help I get this error

--> FOAM Warning :
From function bool Foam::dictionary::add(Foam::entry*, bool)
in file db/dictionary/dictionary.C at line 807
Reading ""
attempt to add entry functions which already exists in dictionary ""
--> FOAM Warning :
From function static bool Foam::functionObjectList::readFunctionObject(const Foam::string&, Foam::dictionary&, Foam::HashSet<>&, const Foam::word&)
in file db/functionObjects/functionObjectList/functionObjectList.C at line 245
Cannot find functionObject file strainRate

ykanani · September 1, 2017, 18:50

Quote:

Originally Posted by pibil1

Hello blebon,

Thanks Can you help me on how to implement this please?, I have copied /opt/openfoam4/src/functionObjects/field/vorticity to /opt/openfoam4/src/functionObjects/field/strainRate. Then replaced everything that says vorticity to strainRate in both strainRate.H and strainRate.C. Then added #include "fvcGrad.H" in strainRate.H and rewrote the calc funcion.

Please help I get this error

--> FOAM Warning :
From function bool Foam::dictionary::add(Foam::entry*, bool)
in file db/dictionary/dictionary.C at line 807
Reading ""
attempt to add entry functions which already exists in dictionary ""
--> FOAM Warning :
From function static bool Foam::functionObjectList::readFunctionObject(const Foam::string&, Foam::dictionary&, Foam::HashSet<>&, const Foam::word&)
in file db/functionObjects/functionObjectList/functionObjectList.C at line 245
Cannot find functionObject file strainRate

Hi, I believe adding the strainRate file under the /opt/openfoam4/etc/caseDicts/postProcessing/fields/ will solve your second warning.
Just copy the vorticity file under that folder and rename it to strainRate. Then modify the file content accordingly. Hope this helps.

Regards,

pibil1 · September 2, 2017, 12:15

Hi Ikanani,

I already had done that, can you help me please? I got this error:

--> FOAM Warning :
From function bool Foam::functionObjectList::read()
in file db/functionObjects/functionObjectList/functionObjectList.C at line 671
Caught FatalError
--> FOAM FATAL ERROR:
Unknown function type strainRate

Valid functions are :

39
(
CourantNo
Lambda2
MachNo
PecletNo
Q
blendingFactor
components
div
enstrophy
fieldAverage
fieldCoordinateSystemTransform
fieldMinMax
fieldValueDelta
flowType
grad
histogram
mag
magSqr
nearWallFields
patchProbes
pressure
probes
processorField
psiReactionThermoMoleFractions
randomise
readFields
regionSizeDistribution
rhoReactionThermoMoleFractions
sets
streamLine
surfaceInterpolate
surfaceRegion
surfaces
turbulenceFields
volRegion
vorticity
wallBoundedStreamLine
wallShearStress
yPlus
)

blebon · September 4, 2017, 09:15

Hi pibil1,

Sorry for the late reply. My additions to the standard code are:

In /etc/caseDicts/postProcessing/fields

file strainRate with contents:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Web:      www.OpenFOAM.org
     \\/     M anipulation  |
-------------------------------------------------------------------------------
Description
    Calculates the strainRate field.

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

type            strainRate;
libs            ("libfieldFunctionObjects.so");

field           U;

executeControl  writeTime;
writeControl    writeTime;

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

In $FOAM_SRC/functionObjects

Modify field/Make/files to add

Code:

strainRate/strainRate.C

just below vorticity/vorticity.C (might be what you are missing?)

Added a folder field/strainRate with contents

strainRate.C

Code:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2014-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

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

#include "strainRate.H"
#include "fvcGrad.H"
#include "addToRunTimeSelectionTable.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace functionObjects
{
    defineTypeNameAndDebug(strainRate, 0);

    addToRunTimeSelectionTable
    (
        functionObject,
        strainRate,
        dictionary
    );
}
}


// * * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * //

bool Foam::functionObjects::strainRate::calc()
{
    if (foundObject<volVectorField>(fieldName_))
    {
        return store
        (
            resultName_,
            sqrt(2.0)*mag(symm(fvc::grad(lookupObject<volVectorField>(fieldName_))))
        );
    }
    else
    {
        return false;
    }

    return true;
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::functionObjects::strainRate::strainRate
(
    const word& name,
    const Time& runTime,
    const dictionary& dict
)
:
    fieldExpression(name, runTime, dict, "U")
{
    setResultName(typeName, "U");
}


// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //

Foam::functionObjects::strainRate::~strainRate()
{}


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

strainRate.H

Code:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2014-2016 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Class
    Foam::functionObjects::strainRate

Group
    grpFieldFunctionObjects

Description
    This function object calculates the strain rate.

See also
    Foam::functionObjects::fieldExpression
    Foam::functionObjects::fvMeshFunctionObject

SourceFiles
    strainRate.C

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

#ifndef functionObjects_strainRate_H
#define functionObjects_strainRate_H

#include "fieldExpression.H"

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

namespace Foam
{
namespace functionObjects
{

/*---------------------------------------------------------------------------*\
                          Class strainRate Declaration
\*---------------------------------------------------------------------------*/

class strainRate
:
    public fieldExpression
{
    // Private Member Functions

        //- Calculate the strainRate field and return true if successful
        virtual bool calc();


public:

    //- Runtime type information
    TypeName("strainRate");


    // Constructors

        //- Construct from Time and dictionary
        strainRate
        (
            const word& name,
            const Time& runTime,
            const dictionary& dict
        );


    //- Destructor
    virtual ~strainRate();
};


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

} // End namespace functionObjects
} // End namespace Foam

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

#endif

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

pibil1 · September 4, 2017, 19:01

Thanks a lot blebon, do I have to compile or make something? because after following step by step your guide I get this error in OpenFOAM 4.1

--> FOAM Warning :
From function bool Foam::dictionary::add(Foam::entry*, bool)
in file db/dictionary/dictionary.C at line 807
Reading "" from line 13 to line 19
attempt to add entry functions which already exists in dictionary ""
--> FOAM Warning :
From function bool Foam::functionObjectList::read()
in file db/functionObjects/functionObjectList/functionObjectList.C at line 671
Caught FatalError
--> FOAM FATAL ERROR:
Unknown function type strainRate

Valid functions are :

39
(
CourantNo
Lambda2
MachNo
PecletNo
Q
blendingFactor
components
div
enstrophy
fieldAverage
fieldCoordinateSystemTransform
fieldMinMax
fieldValueDelta
flowType
grad
histogram
mag
magSqr
nearWallFields
patchProbes
pressure
probes
processorField
psiReactionThermoMoleFractions
randomise
readFields
regionSizeDistribution
rhoReactionThermoMoleFractions
sets
streamLine
surfaceInterpolate
surfaceRegion
surfaces
turbulenceFields
volRegion
vorticity
wallBoundedStreamLine
wallShearStress
yPlus
)

blebon · September 5, 2017, 03:25

Yes, run wmake in $FOAM_SRC/functionObjects/field

pibil1 · September 5, 2017, 12:04

Thank you blebon, you were very helpful

Elham · March 8, 2019, 01:26

Quote:

Originally Posted by pibil1

Thank you blebon, you were very helpful

Hi everybody,

Can I have the stress tensor with postprocessing directly?

I have used foalCalc to have the gradU. The resul is a tensor of 9 elements. I do not know which argument is the Uij and Uji to find the strain tensor then. Anyone knows?

Regards,
Elham

tecmul · April 26, 2019, 12:36

Quote:

Originally Posted by Elham

Hi everybody,

Can I have the stress tensor with postprocessing directly?

I have used foalCalc to have the gradU. The resul is a tensor of 9 elements. I do not know which argument is the Uij and Uji to find the strain tensor then. Anyone knows?

Regards,
Elham

The gradient tensor that gradU outputs is $\partial{u_j}/\partial{x_i}$ . So the first element, grad_0 is $\partial{u}/\partial{x}$ , grad_2 is $\partial{w}/\partial{x}$ and grad_3 is $\partial{u}/\partial{y}$ .

sourav90 · August 9, 2020, 05:57

Quote:

Originally Posted by blebon

Yes, run wmake in $FOAM_SRC/functionObjects/field

For the people who are wondering why it takes so long, try to use:

Code:

wmake -j 16

where `16` is the number of processor cores available in your machine. As noted from here:

HTML Code:

https://www.cfd-online.com/Forums/openfoam-installation/57543-openfoam-14-parallel-build.html

ahparvin · March 4, 2021, 05:32

Quote:

Originally Posted by pibil1

Thanks a lot blebon, do I have to compile or make something? because after following step by step your guide I get this error in OpenFOAM 4.1

--> FOAM Warning :
From function bool Foam::dictionary::add(Foam::entry*, bool)
in file db/dictionary/dictionary.C at line 807
Reading "" from line 13 to line 19
attempt to add entry functions which already exists in dictionary ""
--> FOAM Warning :
From function bool Foam::functionObjectList::read()
in file db/functionObjects/functionObjectList/functionObjectList.C at line 671
Caught FatalError
--> FOAM FATAL ERROR:
Unknown function type strainRate

Valid functions are :

39
(
CourantNo
Lambda2
MachNo
PecletNo
Q
blendingFactor
components
div
enstrophy
fieldAverage
fieldCoordinateSystemTransform
fieldMinMax
fieldValueDelta
flowType
grad
histogram
mag
magSqr
nearWallFields
patchProbes
pressure
probes
processorField
psiReactionThermoMoleFractions
randomise
readFields
regionSizeDistribution
rhoReactionThermoMoleFractions
sets
streamLine
surfaceInterpolate
surfaceRegion
surfaces
turbulenceFields
volRegion
vorticity
wallBoundedStreamLine
wallShearStress
yPlus
)

Hey pibil1

Thank you! I did all steps, The function apparently is running on all time steps, but I can not find any outputs.

I also have warning at the beginning...

Code:

Create time

Create mesh for time = 0

--> FOAM Warning : 
    From function static bool Foam::functionObjectList::readFunctionObject(const Foam::string&, Foam::dictionary&, const Foam::string&, Foam::HashSet<>&, const Foam::word&)
    in file db/functionObjects/functionObjectList/functionObjectList.C at line 311
    Cannot find functionObject file strainRate
Time = 0

Reading fields:


Executing functionObjects

blebon · March 4, 2021, 05:41

Did you put the strainRate dictionary file in the system directory?

ahparvin · March 4, 2021, 08:58

Quote:

Originally Posted by blebon

Did you put the strainRate dictionary file in the system directory?

Thanks for your quick reply!
No, how is that? should I make one?

Tobi · June 13, 2021, 05:45

Hey everybody,

can someone give the information regarding the square root of 2 in front of the equation mentioned in the first post? Based on my derivations (from my book) and here on cfd-online (Calculating divDevReff), I never saw this factor and I have no idea where this factor occurs. For me it seems that the calculation of the strain rate is only used for non-Newtonian fluids and is not related to Newtonian fluids

Tobermory · June 14, 2021, 06:14

I understand your confusion here - in some sources (eg the Shih et al paper on the realizable k-epsilon model, StarCCM+ manual, CFX manual) you'll see the shear rate defined as sqrt(2) times the norm, i.e.:

$\gamma = \sqrt{2 \mathbf{S}:\mathbf{S}}$

but in others (eg Fluent manual for the realizable k-eps model) it will simply be the norm:

$\tilde{S} = \sqrt{\mathbf{S}:\mathbf{S}}$

The reason for the difference is just convention, I think. As I think someone else has said in one of the numerous posts on this subject, the sqrt(2) is introduced for compatibility with the 2D case. Let me explain. Consider a case of a simple shear flow, $\partial U / \partial y$ , with all other velocity partial derivatives being zero. The shear stress is:

$\tau= \mu \frac{\partial U}{\partial y} = \mu \gamma$

where $\gamma = \partial U/\partial y$ is the strain rate. Now, from the strain rate tensor, we have:

$\mathbf{S}_{12} = \mathbf{S}_{21} = \frac{1}{2} \frac{\partial U}{\partial y}$

with all the other components being zero. The norm of this tensor is therefore:

$\sqrt{\mathbf{S}:\mathbf{S}} = \sqrt{\mathbf{S}_{12}^2 + \mathbf{S}_{21}^2} = \sqrt{2\mathbf{S}_{12}^2} =\frac{1}{\sqrt{2}} \frac{\partial U}{\partial y}$

And so to recover the strain rate we need to introduce the sqrt(2) factor:

$\gamma = \sqrt{2\mathbf{S}:\mathbf{S}} = \sqrt{4\mathbf{S}_{12}^2} = \frac{\partial U}{\partial y}$

In other words, in this definition of the strain rate parameter, it is calculated from sqrt(2) times the norm of the strain tensor. Either convention is "correct" - it's just important to keep track of which one you are using.

HPE · June 23, 2021, 17:12

As far as I remember, the global confusion around sqrt(2) thereat stems from FLUENT's unconventional convention, which, for some reason, does not use the factor of 0.5 in the computation of the symmetric part of the gradient tensor, hence affecting the conventional factors in the expressions of the dependent variables, e.g. magnitude of shear rate, in unconventional ways.

Tobermory · June 24, 2021, 03:50

Agreed - that's probably the main cause, although beware that some journal papers, eg the Shih one on the realizable k-epsilon model, will also use the expression without the root 2 (i.e. the $\tilde{S}$ , above) for use in calculating other model parameters (though not to denote the shear rate, which should always have the root 2 I think) ... in fact the Shih paper uses both!

August 9, 2017, 07:47	Function object for strain rate tensor?	#1
blebon Member Bruno Lebon Join Date: Dec 2012 Posts: 33 Rep Power: 13	Dear Foamers, Is there a way of outputting the strain rate using function objects? The strainRate is already calculated in viscosityModel: Code: Foam::tmp<Foam::volScalarField> Foam::viscosityModel::strainRate() const { return sqrt(2.0)*mag(symm(fvc::grad(U_))); } I would like to output this field from a calculated case with -postProcess. Thanks kiski, y_jiang and ahparvin like this.

August 9, 2017, 08:35	Just created a new function object	#2
blebon Member Bruno Lebon Join Date: Dec 2012 Posts: 33 Rep Power: 13	Never mind, found a solution and posting it if anyone interested in the future. Just create a new function object to recalculate the strain rate. Copy the vorticity fn object and rename strainRate, change the curl include line to #include "fvcGrad.H" and edit the calc function as follows: Code: bool Foam::functionObjects::strainRate::calc() { if (foundObject<volVectorField>(fieldName_)) { return store ( resultName_, sqrt(2.0)*mag(symm(fvc::grad(lookupObject<volVectorField>(fieldName_)))) ); } else { return false; } return true; } hulli, rarnaunot, Tanwk and 2 others like this.

September 1, 2017, 18:38	How to achieve	#3
pibil1 New Member Join Date: Aug 2017 Posts: 28 Rep Power: 8	Hello blebon, Thanks Can you help me on how to implement this please?, I have copied /opt/openfoam4/src/functionObjects/field/vorticity to /opt/openfoam4/src/functionObjects/field/strainRate. Then replaced everything that says vorticity to strainRate in both strainRate.H and strainRate.C. Then added #include "fvcGrad.H" in strainRate.H and rewrote the calc funcion. Please help I get this error --> FOAM Warning : From function bool Foam::dictionary::add(Foam::entry*, bool) in file db/dictionary/dictionary.C at line 807 Reading "" attempt to add entry functions which already exists in dictionary "" --> FOAM Warning : From function static bool Foam::functionObjectList::readFunctionObject(const Foam::string&, Foam::dictionary&, Foam::HashSet<>&, const Foam::word&) in file db/functionObjects/functionObjectList/functionObjectList.C at line 245 Cannot find functionObject file strainRate sourav90 likes this.

September 4, 2017, 19:01		#7
pibil1 New Member Join Date: Aug 2017 Posts: 28 Rep Power: 8	Thanks a lot blebon, do I have to compile or make something? because after following step by step your guide I get this error in OpenFOAM 4.1 --> FOAM Warning : From function bool Foam::dictionary::add(Foam::entry*, bool) in file db/dictionary/dictionary.C at line 807 Reading "" from line 13 to line 19 attempt to add entry functions which already exists in dictionary "" --> FOAM Warning : From function bool Foam::functionObjectList::read() in file db/functionObjects/functionObjectList/functionObjectList.C at line 671 Caught FatalError --> FOAM FATAL ERROR: Unknown function type strainRate Valid functions are : 39 ( CourantNo Lambda2 MachNo PecletNo Q blendingFactor components div enstrophy fieldAverage fieldCoordinateSystemTransform fieldMinMax fieldValueDelta flowType grad histogram mag magSqr nearWallFields patchProbes pressure probes processorField psiReactionThermoMoleFractions randomise readFields regionSizeDistribution rhoReactionThermoMoleFractions sets streamLine surfaceInterpolate surfaceRegion surfaces turbulenceFields volRegion vorticity wallBoundedStreamLine wallShearStress yPlus ) sourav90 likes this.

September 5, 2017, 03:25		#8
blebon Member Bruno Lebon Join Date: Dec 2012 Posts: 33 Rep Power: 13	Yes, run wmake in $FOAM_SRC/functionObjects/field hulli, pibil1 and sourav90 like this.

September 2, 2017, 12:15		#5
pibil1 New Member Join Date: Aug 2017 Posts: 28 Rep Power: 8	Hi Ikanani, I already had done that, can you help me please? I got this error: --> FOAM Warning : From function bool Foam::functionObjectList::read() in file db/functionObjects/functionObjectList/functionObjectList.C at line 671 Caught FatalError --> FOAM FATAL ERROR: Unknown function type strainRate Valid functions are : 39 ( CourantNo Lambda2 MachNo PecletNo Q blendingFactor components div enstrophy fieldAverage fieldCoordinateSystemTransform fieldMinMax fieldValueDelta flowType grad histogram mag magSqr nearWallFields patchProbes pressure probes processorField psiReactionThermoMoleFractions randomise readFields regionSizeDistribution rhoReactionThermoMoleFractions sets streamLine surfaceInterpolate surfaceRegion surfaces turbulenceFields volRegion vorticity wallBoundedStreamLine wallShearStress yPlus )

September 5, 2017, 12:04		#9
pibil1 New Member Join Date: Aug 2017 Posts: 28 Rep Power: 8	Thank you blebon, you were very helpful

March 4, 2021, 05:41		#14
blebon Member Bruno Lebon Join Date: Dec 2012 Posts: 33 Rep Power: 13	Did you put the strainRate dictionary file in the system directory?

June 13, 2021, 05:45		#16
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hey everybody, can someone give the information regarding the square root of 2 in front of the equation mentioned in the first post? Based on my derivations (from my book) and here on cfd-online (Calculating divDevReff), I never saw this factor and I have no idea where this factor occurs. For me it seems that the calculation of the strain rate is only used for non-Newtonian fluids and is not related to Newtonian fluids __________________ Keep foaming, Tobias Holzmann

June 14, 2021, 06:14		#17
Tobermory Senior Member Join Date: Apr 2020 Location: UK Posts: 668 Rep Power: 14	I understand your confusion here - in some sources (eg the Shih et al paper on the realizable k-epsilon model, StarCCM+ manual, CFX manual) you'll see the shear rate defined as sqrt(2) times the norm, i.e.: $\gamma = \sqrt{2 \mathbf{S}:\mathbf{S}}$ but in others (eg Fluent manual for the realizable k-eps model) it will simply be the norm: $\tilde{S} = \sqrt{\mathbf{S}:\mathbf{S}}$ The reason for the difference is just convention, I think. As I think someone else has said in one of the numerous posts on this subject, the sqrt(2) is introduced for compatibility with the 2D case. Let me explain. Consider a case of a simple shear flow, $\partial U / \partial y$ , with all other velocity partial derivatives being zero. The shear stress is: $\tau= \mu \frac{\partial U}{\partial y} = \mu \gamma$ where $\gamma = \partial U/\partial y$ is the strain rate. Now, from the strain rate tensor, we have: $\mathbf{S}_{12} = \mathbf{S}_{21} = \frac{1}{2} \frac{\partial U}{\partial y}$ with all the other components being zero. The norm of this tensor is therefore: $\sqrt{\mathbf{S}:\mathbf{S}} = \sqrt{\mathbf{S}_{12}^2 + \mathbf{S}_{21}^2} = \sqrt{2\mathbf{S}_{12}^2} =\frac{1}{\sqrt{2}} \frac{\partial U}{\partial y}$ And so to recover the strain rate we need to introduce the sqrt(2) factor: $\gamma = \sqrt{2\mathbf{S}:\mathbf{S}} = \sqrt{4\mathbf{S}_{12}^2} = \frac{\partial U}{\partial y}$ In other words, in this definition of the strain rate parameter, it is calculated from sqrt(2) times the norm of the strain tensor. Either convention is "correct" - it's just important to keep track of which one you are using. HPE and ahparvin like this.

June 23, 2021, 17:12		#18
HPE Senior Member Herpes Free Engineer Join Date: Sep 2019 Location: The Home Under The Ground with the Lost Boys Posts: 932 Rep Power: 12	As far as I remember, the global confusion around sqrt(2) thereat stems from FLUENT's unconventional convention, which, for some reason, does not use the factor of 0.5 in the computation of the symmetric part of the gradient tensor, hence affecting the conventional factors in the expressions of the dependent variables, e.g. magnitude of shear rate, in unconventional ways. __________________ The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror

June 24, 2021, 03:50		#19
Tobermory Senior Member Join Date: Apr 2020 Location: UK Posts: 668 Rep Power: 14	Agreed - that's probably the main cause, although beware that some journal papers, eg the Shih one on the realizable k-epsilon model, will also use the expression without the root 2 (i.e. the $\tilde{S}$ , above) for use in calculating other model parameters (though not to denote the shear rate, which should always have the root 2 I think) ... in fact the Shih paper uses both!

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Mass Flow Rate Custom Field Function	AJoubert	FLUENT	2	March 23, 2013 08:50
OpenFOAM static build on Cray XT5	asaijo	OpenFOAM Installation	9	April 6, 2011 12:21
[blockMesh] BlockMesh FOAM warning	gaottino	OpenFOAM Meshing & Mesh Conversion	7	July 19, 2010 14:11
Compilation errors in ThirdPartymallochoard	feng_w	OpenFOAM Installation	1	January 25, 2009 06:59
[blockMesh] BlockMeshmergePatchPairs	hjasak	OpenFOAM Meshing & Mesh Conversion	11	August 15, 2008 07:36