[sourav90]

Dear All,

I want to calculate/visualise shear stress inside the fluid domain. I came through wallShearStress utility but as you know, it only calculates the shear stress at the wall.

My model is very simple: a long pipe, with a non-Newtonian fluid simulated at a certain pressure difference between the inlet and the outlet, solved using simpleFoam.

Surprisingly, I found no relevant documentation, although there is plenty of discussion regarding the shear stress at the wall. I came through this helpful post, which enabled me to calculate shear strain in the fluid domain but finding it hard to adopt the approach to obtain shear stress.

Function object for strain rate tensor?

I tried with the approach mentioned there, by making files named fluidShearStressSM.C etc. At the wmake stage it throws a lot of errors such as :

g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam7/src/finiteVolume/lnInclude -I/opt/openfoam7/src/meshTools/lnInclude -I/opt/openfoam7/src/lagrangian/basic/lnInclude -I/opt/openfoam7/src/fileFormats/lnInclude -I/opt/openfoam7/src/sampling/lnInclude -I/opt/openfoam7/src/surfMesh/lnInclude -I/opt/openfoam7/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam7/src/thermophysicalModels/solidThermo/lnInclude -I/opt/openfoam7/src/transportModels -I/opt/openfoam7/src/transportModels/compressible/lnInclude -I/opt/openfoam7/src/TurbulenceModels/turbulenceModels/lnInclude -I/opt/openfoam7/src/TurbulenceModels/incompressible/lnInclude -I/opt/openfoam7/src/TurbulenceModels/compressible/lnInclude -IlnInclude -I. -I/opt/openfoam7/src/OpenFOAM/lnInclude -I/opt/openfoam7/src/OSspecific/POSIX/lnInclude   -fPIC -c fluidShearStressSM/fluidShearStressSM.C -o /opt/openfoam7/platforms/linux64GccDPInt32Opt/src/functionObjects/field/fluidShearStressSM/fluidShearStressSM.o
fluidShearStressSM/fluidShearStressSM.C: In member function ‘virtual bool Foam::functionObjects::fluidShearStressSM::calc()’:
fluidShearStressSM/fluidShearStressSM.C:65:13: error: expected primary-expression before ‘const’
   65 |             const volTensorField& gradU = fvc::grad(U);
      |             ^~~~~
fluidShearStressSM/fluidShearStressSM.C:68:43: error: ‘mu’ was not declared in this scope
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                           ^~
fluidShearStressSM/fluidShearStressSM.C:68:49: error: ‘gradU’ was not declared in this scope
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                                 ^~~~~
fluidShearStressSM/fluidShearStressSM.C:69:9: error: expected primary-expression before ‘)’ token
   69 |         );
      |         ^
fluidShearStressSM/fluidShearStressSM.C:68:35: warning: unused variable ‘tau’ [-Wunused-variable]
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                   ^~~
fluidShearStressSM/fluidShearStressSM.C: In constructor ‘Foam::functionObjects::fluidShearStressSM::fluidShearStressSM(const Foam::word&, const Foam::Time&, const Foam::dictionary&)’:
fluidShearStressSM/fluidShearStressSM.C:90:5: error: type ‘Foam::functionObjects::fvMeshFunctionObject’ is not a direct base of ‘Foam::functionObjects::fluidShearStressSM’
   90 |     fvMeshFunctionObject(name, runTime, dict),
      |     ^~~~~~~~~~~~~~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:91:5: error: class ‘Foam::functionObjects::fluidShearStressSM’ does not have any field named ‘logFiles’
   91 |     logFiles(obr_, name),
      |     ^~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:92:5: error: class ‘Foam::functionObjects::fluidShearStressSM’ does not have any field named ‘writeLocalObjects’
   92 |     writeLocalObjects(obr_, log),
      |     ^~~~~~~~~~~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:93:1: error: expected identifier before ‘{’ token
   93 | {
      | ^
fluidShearStressSM/fluidShearStressSM.C:93:1: error: no matching function for call to ‘Foam::functionObjects::fieldExpression::fieldExpression()’
In file included from fluidShearStressSM/fluidShearStressSM.H:42,
                 from fluidShearStressSM/fluidShearStressSM.C:26:
lnInclude/fieldExpression.H:88:9: note: candidate: ‘Foam::functionObjects::fieldExpression::fieldExpression(const Foam::word&, const Foam::Time&, const Foam::dictionary&, const Foam::word&, const Foam::word&)’
   88 |         fieldExpression
      |         ^~~~~~~~~~~~~~~
lnInclude/fieldExpression.H:88:9: note:   candidate expects 5 arguments, 0 provided
fluidShearStressSM/fluidShearStressSM.C:95:5: error: ‘resetName’ was not declared in this scope; did you mean ‘resultName_’?
   95 |     resetName(typeName);
      |     ^~~~~~~~~
      |     resultName_
fluidShearStressSM/fluidShearStressSM.C:96:5: error: ‘resetLocalObjectName’ was not declared in this scope
   96 |     resetLocalObjectName(typeName);
      |     ^~~~~~~~~~~~~~~~~~~~
make: *** [/opt/openfoam7/wmake/rules/General/transform:26: /opt/openfoam7/platforms/linux64GccDPInt32Opt/src/functionObjects/field/fluidShearStressSM/fluidShearStressSM.o] Error 1

I would like to have the code usable both as a runtime or a post-processing tool.

I am new to OpenFOAM & have no prior exposure to OOC++ coding. Any suggestion or pointers in the right direction would help me greatly in my research, with this nice open-source software.

[fanta]

-Move to $FOAM_SRC/etc/caseDicts/postProcessing/fields
-make a copy of vorticity to strainRate, replace every occurance of vorticity with strainRate in the files
-Move to $FOAM_SRC/functionObjects/field/make. Edit "files", add strainRate/strainRate.C after vorticity
-copy the folder vorticity in $FOAM_SRC/functionObjects/field to strainRate
-replace vorticity with strainRate in the copied filenames
-in strainRate.C replace #fvcCurl.H with #fvcGrad.H, replace function calc() with

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

    return false;

For non-Newtonian Liquids this formula is generally wrong. I could not find a better approach, yet.

[sourav90]

Originally Posted by fanta

For non-Newtonian Liquids this formula is generally wrong. I could not find a better approach, yet.

Why is the formula generally wrong?

BTW, the problem I am facing isn't with implementing strain rate (it works as that link says), rather with the shear stress in the entire fluid domain. Sorry, if I wasn't clear enough...

[sourav90]

I found a workaround while fiddling with Swak4Foam. He files or commands that I used are as follow:

• Contents of `funkySetFieldsDict`, to be placed inside `system/`

FoamFile
{
    version         2.0;
    format          ascii;
    instance        "system";
    local           "";
    class           dictionary;
    object          funkySetFieldsDict;
}

expressions (
    setTau {
        field           Tau;
        create          true ;
        expression      "mag(grad(U))*nu";
    }
);

• After the simulation was over, I ran

  funkySetFields -time '500:3000'

The simulation is as such that the highest shear stress would be at the wall. So, I compare the maximum values of shear stress and wall shear stress (using the wallShearStress utility), it's hugely different. I am not sure now, which one is correct. Can anybody help me inferring where is the error?

[Bodo1993]

Hi Sourav,
I am wondering if you managed to get a way to extract the correct stress tensor from the openFoam simulations. Thanks.

[sourav90]

Hello Bodo1993, if you haven't found it already there are two ways to achieve this.

First, with OpenFOAM version 8, you can just add these lines at the end of your controldict file:

functions
{
//https://www.openfoam.com/documentation/guides/latest/doc/guide-function-objects.html
    #includeFunc            shearStress;

}

Copying the commit notes from here https://github.com/OpenFOAM/OpenFOAM...ae08a224cc9d4b

"MomentumTransportModels: Update of the TurbulenceModels library for a…
…ll flow types

providing the shear-stress term in the momentum equation for incompressible and
compressible Newtonian, non-Newtonian and visco-elastic laminar flow as well as
Reynolds averaged and large-eddy simulation of turbulent flow.

The general deviatoric shear-stress term provided by the MomentumTransportModels
library is named divDevTau for compressible flow and divDevSigma (sigma =
tau/rho) for incompressible flow, the spherical part of the shear-stress is
assumed to be either included in the pressure or handled separately. The
corresponding stress function sigma is also provided which in the case of
Reynolds stress closure returns the effective Reynolds stress (including the
laminar contribution) or for other Reynolds averaged or large-eddy turbulence
closures returns the modelled Reynolds stress or sub-grid stress respectively.
For visco-elastic flow the sigma function returns the effective total stress
including the visco-elastic and Newtonian contributions.

For thermal flow the heat-flux generated by thermal diffusion is now handled by
the separate ThermophysicalTransportModels library allowing independent run-time
selection of the heat-flux model.

During the development of the MomentumTransportModels library significant effort
has been put into rationalising the components and supporting libraries,
removing redundant code, updating names to provide a more logical, consistent
and extensible interface and aid further development and maintenance. All
solvers and tutorials have been updated correspondingly and backward
compatibility of the input dictionaries provided.

Henry G. Weller
CFD Direct Ltd."

Second, iff you are curious, have time & want to have fun, then you can implement this yourself, with the cue from here Function object for strain rate tensor? However, this leads to some naming issue with the recent versions, due to the changes described here https://github.com/OpenFOAM/OpenFOAM...6bca16c6020bfe. If anyone try this with the new versions & it works, it would be great if you share it

[Beta Liu]

I have a similar problem, would you like to ask if it is solved? If solved, can you share the code for calculating fluid shear stress? I would be very grateful and happy to share it. Thanks!

Originally Posted by sourav90

Dear All,

I want to calculate/visualise shear stress inside the fluid domain. I came through wallShearStress utility but as you know, it only calculates the shear stress at the wall.

My model is very simple: a long pipe, with a non-Newtonian fluid simulated at a certain pressure difference between the inlet and the outlet, solved using simpleFoam.

Surprisingly, I found no relevant documentation, although there is plenty of discussion regarding the shear stress at the wall. I came through this helpful post, which enabled me to calculate shear strain in the fluid domain but finding it hard to adopt the approach to obtain shear stress.

Function object for strain rate tensor?

I tried with the approach mentioned there, by making files named fluidShearStressSM.C etc. At the wmake stage it throws a lot of errors such as :

g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam7/src/finiteVolume/lnInclude -I/opt/openfoam7/src/meshTools/lnInclude -I/opt/openfoam7/src/lagrangian/basic/lnInclude -I/opt/openfoam7/src/fileFormats/lnInclude -I/opt/openfoam7/src/sampling/lnInclude -I/opt/openfoam7/src/surfMesh/lnInclude -I/opt/openfoam7/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam7/src/thermophysicalModels/solidThermo/lnInclude -I/opt/openfoam7/src/transportModels -I/opt/openfoam7/src/transportModels/compressible/lnInclude -I/opt/openfoam7/src/TurbulenceModels/turbulenceModels/lnInclude -I/opt/openfoam7/src/TurbulenceModels/incompressible/lnInclude -I/opt/openfoam7/src/TurbulenceModels/compressible/lnInclude -IlnInclude -I. -I/opt/openfoam7/src/OpenFOAM/lnInclude -I/opt/openfoam7/src/OSspecific/POSIX/lnInclude   -fPIC -c fluidShearStressSM/fluidShearStressSM.C -o /opt/openfoam7/platforms/linux64GccDPInt32Opt/src/functionObjects/field/fluidShearStressSM/fluidShearStressSM.o
fluidShearStressSM/fluidShearStressSM.C: In member function ‘virtual bool Foam::functionObjects::fluidShearStressSM::calc()’:
fluidShearStressSM/fluidShearStressSM.C:65:13: error: expected primary-expression before ‘const’
   65 |             const volTensorField& gradU = fvc::grad(U);
      |             ^~~~~
fluidShearStressSM/fluidShearStressSM.C:68:43: error: ‘mu’ was not declared in this scope
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                           ^~
fluidShearStressSM/fluidShearStressSM.C:68:49: error: ‘gradU’ was not declared in this scope
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                                 ^~~~~
fluidShearStressSM/fluidShearStressSM.C:69:9: error: expected primary-expression before ‘)’ token
   69 |         );
      |         ^
fluidShearStressSM/fluidShearStressSM.C:68:35: warning: unused variable ‘tau’ [-Wunused-variable]
   68 |             const volTensorField& tau = - mu * (gradU + gradU.T());
      |                                   ^~~
fluidShearStressSM/fluidShearStressSM.C: In constructor ‘Foam::functionObjects::fluidShearStressSM::fluidShearStressSM(const Foam::word&, const Foam::Time&, const Foam::dictionary&)’:
fluidShearStressSM/fluidShearStressSM.C:90:5: error: type ‘Foam::functionObjects::fvMeshFunctionObject’ is not a direct base of ‘Foam::functionObjects::fluidShearStressSM’
   90 |     fvMeshFunctionObject(name, runTime, dict),
      |     ^~~~~~~~~~~~~~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:91:5: error: class ‘Foam::functionObjects::fluidShearStressSM’ does not have any field named ‘logFiles’
   91 |     logFiles(obr_, name),
      |     ^~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:92:5: error: class ‘Foam::functionObjects::fluidShearStressSM’ does not have any field named ‘writeLocalObjects’
   92 |     writeLocalObjects(obr_, log),
      |     ^~~~~~~~~~~~~~~~~
fluidShearStressSM/fluidShearStressSM.C:93:1: error: expected identifier before ‘{’ token
   93 | {
      | ^
fluidShearStressSM/fluidShearStressSM.C:93:1: error: no matching function for call to ‘Foam::functionObjects::fieldExpression::fieldExpression()’
In file included from fluidShearStressSM/fluidShearStressSM.H:42,
                 from fluidShearStressSM/fluidShearStressSM.C:26:
lnInclude/fieldExpression.H:88:9: note: candidate: ‘Foam::functionObjects::fieldExpression::fieldExpression(const Foam::word&, const Foam::Time&, const Foam::dictionary&, const Foam::word&, const Foam::word&)’
   88 |         fieldExpression
      |         ^~~~~~~~~~~~~~~
lnInclude/fieldExpression.H:88:9: note:   candidate expects 5 arguments, 0 provided
fluidShearStressSM/fluidShearStressSM.C:95:5: error: ‘resetName’ was not declared in this scope; did you mean ‘resultName_’?
   95 |     resetName(typeName);
      |     ^~~~~~~~~
      |     resultName_
fluidShearStressSM/fluidShearStressSM.C:96:5: error: ‘resetLocalObjectName’ was not declared in this scope
   96 |     resetLocalObjectName(typeName);
      |     ^~~~~~~~~~~~~~~~~~~~
make: *** [/opt/openfoam7/wmake/rules/General/transform:26: /opt/openfoam7/platforms/linux64GccDPInt32Opt/src/functionObjects/field/fluidShearStressSM/fluidShearStressSM.o] Error 1

I would like to have the code usable both as a runtime or a post-processing tool.

I am new to OpenFOAM & have no prior exposure to OOC++ coding. Any suggestion or pointers in the right direction would help me greatly in my research, with this nice open-source software.

[sourav90]

Originally Posted by Beta Liu

I have a similar problem, would you like to ask if it is solved? If solved, can you share the code for calculating fluid shear stress? I would be very grateful and happy to share it. Thanks!

Sorry for my late reply! My goal was to plot the shear stress in the entire domain -wallShearStress utility (functionObject) wasn't good for that. I used the OpenFOAM.org (version 6) back then. Later on OpenFOAM 7/8 provided shearStress utility, which served the purpose

You can find a minimal reproducible example (MRE), for the published paper with this work here: inSilicoE3DBP_model_MRE

[chaudhad]

Hi Sourav and everyone,


I know this is an ancient post but I hope someone can find me a solution. I have been stuck for a very long time. I am actually doing LES and cannot figure out how to output wall shear stress during the simulation in openfoam. So I was trying to calculate the wall shear stress in Paraview using gradientOfUnstructuresDataSet and then extracting the surface and computing the surface normals and then doing the dot product of this gradient tensor with the surface normal vector and the dynamic viscosity to calculate the wall shear stress. But my gradient vectors are computed all zero on the wall. I don't know how to include the gradient at the cell centroid and not at the face of the wall cell. Any help will be highly appreciated.