y+ and u+ values with low-Re RANS turbulence models: utility + testcase

HanSolo123 · May 11, 2014, 08:13

Hello,

I have the same problem like aylalisa. The post-Processing utility "wallShearStress" actually only works for RANS-Simulation. I actually dont understand why it is so but ok.

I found a thread here on the forum how to calculate the wall shear stress tau_w for LES(
http://www.cfd-online.com/Forums/ope...imulation.html )
but this does not work for OP2.3.0 anymore. I had a look in wallShearStress.C, but there is no reference to #include "incompressible/RAS/RASModel/RASModel.H" anymore as mentioned in the above thread.

I want to plot u+ over y+ as well, therefor I need u+. When I extract u_tau from y+, is it possible to calculate u+ then with
u+ = u / u_tau?

I am unsure about the directions. In which direction points u_tau, when you have a simple Channel flow in x-direction? When I extract it from y+, does it point in x-direction then? The u+ over y+ graph is actually a dimensionless velocity profile, so it is velocity in x over wall distance in y. But i am unsure about u_tau.
Any tips?

ArathoN · May 11, 2014, 13:22

Quote:

Originally Posted by HanSolo123

Hello,

I have the same problem like aylalisa. The post-Processing utility "wallShearStress" actually only works for RANS-Simulation. I actually dont understand why it is so but ok.

I found a thread here on the forum how to calculate the wall shear stress tau_w for LES(
http://www.cfd-online.com/Forums/ope...imulation.html )
but this does not work for OP2.3.0 anymore. I had a look in wallShearStress.C, but there is no reference to #include "incompressible/RAS/RASModel/RASModel.H" anymore as mentioned in the above thread.

I want to plot u+ over y+ as well, therefor I need u+. When I extract u_tau from y+, is it possible to calculate u+ then with
u+ = u / u_tau?

I am unsure about the directions. In which direction points u_tau, when you have a simple Channel flow in x-direction? When I extract it from y+, does it point in x-direction then? The u+ over y+ graph is actually a dimensionless velocity profile, so it is velocity in x over wall distance in y. But i am unsure about u_tau.
Any tips?

Here my answer to the same question about u+ vs y+ calculation.

The u_tau calculated is the magnitude of the friction velocity utau (u_taux, u_tauy , u_tauz); same thing for the wallshearstress. Obviously if you study a 1-D case the values over that direction are the ones to study hence their value over the other 2 directions are negligeble.

adambarfi · May 22, 2014, 01:11

hi,

I have some problem in making compressibleyPlusLES utility.
when I want to make it the following error is appeared:

Code:

In file included from compressibleyPlusLES.C:70:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:112:57: error: no matching function for call to ‘Foam::compressible::LESModel::New(Foam::volScalarField&, Foam::volVectorField&, Foam::surfaceScalarField&, Foam::basicThermo&)’
createFields.H:112:57: note: candidate is:
/home/mostafa/OpenFOAM/OpenFOAM-2.2.2/src/turbulenceModels/compressible/LES/LESModel/LESModel.H:150:34: note: static Foam::autoPtr<Foam::compressible::LESModel> Foam::compressible::LESModel::New(const volScalarField&, const volVectorField&, const surfaceScalarField&, const Foam::fluidThermo&, const Foam::word&)
/home/mostafa/OpenFOAM/OpenFOAM-2.2.2/src/turbulenceModels/compressible/LES/LESModel/LESModel.H:150:34: note:   no known conversion for argument 4 from ‘Foam::basicThermo’ to ‘const Foam::fluidThermo&’
make: *** [Make/linux64GccDPOpt/compressibleyPlusLES.o] Error 1

anybody knows what should I do?

Regards,
Mostafa

Edit: I'm using OF-2.2.2

adambarfi · May 22, 2014, 02:24

Hi dear FOAMERs, specially LES fans!

I decided to change the compressibleyPlusLES to incompressibleyPlusLES utility. I made the changes and fortunately it was made without any errors.
I attach the final utility and if it's possible for you guys to check it and if I made some mistakes in writing the codes, please let me know.

Regards,
Mostafa

New_OpenFOAM_user · September 9, 2014, 14:23

Quote:

Originally Posted by lakeat

Hey guys,

1. I found calculate wall distance twice is unnecessary, so I disable it.
2. Here are the two utilities doing the same job as before, with small changes. Tested on OpenFOAM-2.2.x
3. I have also added a few write-out control.

Please use "-help" to find more info.

yPlus: Attachment 26083
yStar: Attachment 26084

Hi,

Thank you for continually updating and uploading your utility for newer versions of OF.

I have a question about your utility. Please forgive if it is an ignorant question, but I haven't been able to find the answers elsewhere. I read that you wrote it for low Re numbers, is it valid for high Re turbulence models (in my case realizable k-eps)?

Also when I build and run your utility (in OF version 2.3.x) it only displays the yPlus values for one of my patches and the value displayed is much lower than the y* values calculated by the yPlusRAS utility. Is it working correctly, or could you suggest how to modify it? Or is there something else I am missing?

Thank youin advance, your help is greatly appreciated!
Chrissy.

ArathoN · October 15, 2014, 13:06

Quote:

Originally Posted by New_OpenFOAM_user

.................................

yplus and ystar have different relations so they will obviously give different values. They have a comparable results only in the log layer because the assumption to define ystar depends on the log layer.

this utility gives the possibility to calculate yplus when you are using a wall resolved case where nut at wall must be set as calculated. However the yPlusRAS calculate yplus only if it is declared a nutWallFunction (whatever it is) so for the wall resolved case, it will give you errors and no yplus will be clculated.

For high Re meshes use teh yPlusRAS included in OF, take care on how it is defined yplus in the wallfunction, because the utility yPlusRAS does only call the function to calculate yplus inside the nutWallFunction chosen in /0/nut. Some of them use ystar others not, I Advice you to read teh code and you'll understand better (see the unige and chalmers course for OF they are really good).

Alhasan · January 13, 2015, 15:13

Quote:

Originally Posted by lakeat

Hi again,

I think I have fixed the bug.

yPlus utility: Attachment 17317
yStar utility: Attachment 17318

Equations used for incompressible flow:

Code:

y^+=\frac{y\sqrt{\frac{\mu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}{\rho}}}{\frac{\mu_{lam}}{\rho}}=\frac{y\sqrt{{\nu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}}}{\nu_{lam}}

Equations used for compressible flow:

Code:

y^+=\frac{y\sqrt{\frac{\mu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}{\rho}}}{\frac{\mu_{lam}}{\rho}}=\frac{y\sqrt{\rho{\mu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}}}{\mu_{lam}}

Hello I beleive this is for OpenFOAM V2.1.0
but when I try to compile I am getting this error

Code:

Making dependency list for source file yPlus.C
SOURCE=yPlus.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/meshTools/lnInclude -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/turbulenceModels -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/transportModels -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/thermophysicalModels/basic/lnInclude -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude -IlnInclude -I. -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude -I/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/yPlus.o
yPlus.C: In function ‘int main(int, char**)’:
yPlus.C:160:38: error: no matching function for call to ‘Foam::basicThermo::New(Foam::fvMesh&)’
yPlus.C:160:38: note: candidate is:
/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/dictionary.H:238:36: note: static Foam::autoPtr<Foam::dictionary> Foam::dictionary::New(Foam::Istream&)
/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/dictionary.H:238:36: note:   no known conversion for argument 1 from ‘Foam::fvMesh’ to ‘Foam::Istream&’
yPlus.C:222:46: error: no matching function for call to ‘Foam::basicThermo::New(Foam::fvMesh&)’
yPlus.C:222:46: note: candidate is:
/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/dictionary.H:238:36: note: static Foam::autoPtr<Foam::dictionary> Foam::dictionary::New(Foam::Istream&)
/users/mk14466/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/dictionary.H:238:36: note:   no known conversion for argument 1 from ‘Foam::fvMesh’ to ‘Foam::Istream&’
make: *** [Make/linux64GccDPOpt/yPlus.o] Error 1

What is happening here

Thanks for your time,
Hasan K.J

hamsteri15 · March 14, 2015, 10:21

I have a question about the plusPostRANS utility. If I understood correctly, the average(uTauWall) function calculates the wall-average of u_tau. So for a flat plate flow ,for example, if I wanted to plot the dimensionless velocity profile at certain x-coordinate location using the u+ and y+ values output from the utility, the values are actually quite far off?

Has anyone come up with a nice way to plot the accurate dimensionless velocity profile with low-Re models? So far I've always calculated the u+ and y+ manually using the velocity gradient (wallGradU) at certain point but for more complex geometries this is quite tedious.

Is it possible to modify the utility so that it uses the same location for the surface normal gradient of the velocity and the point at the wall it calculates the distance to?

KateEisenhower · June 9, 2015, 09:13

Quote:

Originally Posted by lakeat

Hey guys,

1. I found calculate wall distance twice is unnecessary, so I disable it.
2. Here are the two utilities doing the same job as before, with small changes. Tested on OpenFOAM-2.2.x
3. I have also added a few write-out control.

Please use "-help" to find more info.

yPlus: Attachment 26083
yStar: Attachment 26084

Hello,

when I try to compile it I get the attached output.

I'm running OpenFOAM 2.3.1 on OS X Yosemite. I'd appreciate it if anyone could answer my questions:

1) Has anyone successfully compiled the tool on 2.3.x?
2) What is the compiler complaining about?
3) How can I make it work?

Best regards,

Kate

Astrodan · March 24, 2016, 08:36

Quote:

Originally Posted by lakeat

Equations used for compressible flow:

Code:

y^+=\frac{y\sqrt{\frac{\mu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}{\rho}}}{\frac{\mu_{lam}}{\rho}}=\frac{y\sqrt{\rho{\mu_{eff}\left(\frac{\partial U}{\partial y}\right)_{y=0}}}}{\mu_{lam}}

Although this might be true, you apparently also changed the calculation of $u_\tau$ , which appears to be wrong:

$u_\tau = \sqrt{\frac{\tau_w}{\rho}} = \sqrt{\frac{\mu_{eff} \left(\frac{\partial U}{\partial y}\right)_{y=0}}{\rho}}$

while your current code (line 314 [(int) pi*100, yeah])

$u_\tau = \sqrt{\rho \cdot \mu_{eff} \left(\frac{\partial U}{\partial y}\right)_{y=0}}$

The fact that

has the $\rho$ in the nominator is due to the $\nu$ in the nominator of the

-Equation:

$y^+ = \frac{u_\tau y}{\nu} = \frac{u_\tau y \cdot \rho}{\mu}$

At least that's my take at those equations. Maybe someone should re-check, I got a bit confused with all the mu, nu, muEff, nuEff, y+ and y* reading.
Anyway, thanks for the utility, works great so far (tested with 2.3.x).

Astrodan · April 21, 2016, 12:54

Hi there, me again.

For whoever is interested, I updated lakeat's code with the above mentioned correction for $u_{\tau}$ , since so far no one complained. Apart from that I added a -newTimes option, which is just like the -newTimes option in reconstructPar. And finally I update the Make/files to build the tool in the FOAM_USER_APPBIN, not in the global one, so it can be compiled by everyone.

Tested with OF 2.3.x. Both tools in one package. And zipped. I hate .tar.gz.

gu1 · April 28, 2018, 10:35

Quote:

Originally Posted by florian_krause

Dear all,

This issue was already discussed in some length in various threads. Therefore I finally reviewed and attached my plusPostRANS utility.

It calculates y+ and u+ values when using one of the available low-Re RANS turbulence models. I hope the code as well as the output will be self-explaining

I also attached a case. It is a straight pipe (wedge) with periodic inlet/outlet boundary conditions. The Reynolds number based on the mean axial velocity is Re=5300. You can run the case using pisoFoam.

I would appreciate any feedback, it might be still improved at some point!

Best regards,
Florian

Hi, can you help me?!
ERRO:

Quote:

OpenFOAM/plusPostRANS$ wmake all
g++ -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 -O3 -DNoRepository -ftemplate-depth-100 -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/meshTools/lnInclude -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/TurbulenceModels/turbulenceModels/lnInclude -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/TurbulenceModels/turbulenceModels/RAS/RASModel -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/TurbulenceModels/turbulenceModels/LES/LESModel -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/TurbulenceModels/turbulenceModels/LES/LESdeltas/lnInclude -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/transportModels -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/OpenFOAM/lnInclude -I/home/cae/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/lnInclude -fPIC -c plusPostRANS.C -o Make/linux64GccDPInt32Opt/plusPostRANS.o
In file included from plusPostRANS.C:76:0:
createFields.H: In function ‘int main(int, char**)’:
createFields.H:75:10: error: ‘incompressible’ was not declared in this scope
autoPtr<incompressible::RASModel> RASModel
^
createFields.H:75:34: error: template argument 1 is invalid
autoPtr<incompressible::RASModel> RASModel
^
createFields.H:77:13: error: ‘incompressible’ is not a class or namespace
incompressible::RASModel::New(U, phi, laminarTransport)
^
plusPostRANS.C:90:45: error: ‘wallFvPatch’ was not declared in this scope
if (typeid(currPatch) == typeid(wallFvPatch))
^
plusPostRANS.C:96:33: error: base operand of ‘->’ is not a pointer
RASModel->nu().boundaryField()[patchi]
^
plusPostRANS.C:99:29: error: base operand of ‘->’ is not a pointer
/RASModel->nu().boundaryField()[patchi];
^
plusPostRANS.C:106:15: error: base operand of ‘->’ is not a pointer
RASModel->nu()
^
plusPostRANS.C:131:43: error: base operand of ‘->’ is not a pointer
yPlus = y.y() * uTauAvg / RASModel->nu();
^
/home/cae/OpenFOAM/OpenFOAM-3.0.x/wmake/rules/General/transform:8: recipe for target 'Make/linux64GccDPInt32Opt/plusPostRANS.o' failed
make: *** [Make/linux64GccDPInt32Opt/plusPostRANS.o] Error 1

wouter · May 4, 2018, 10:09

Hello gu1,
The utility was written for OF2.3.x. So compiling for OF3.0 can give problems. I cannot help you solve it, but you can download OF2.3.x and use that to run your model and the utility or you can find out what changed between OF2.3 and OF3.0 and adapt the utility to OF3.0 (please post the adapted utility if you do).

Best regards,
Wouter

calf.Z · June 25, 2019, 01:58

how can I plot y+ and u+ in OpenFOAM. Dose anyone modify the tools? Thank you.

fly_light · August 23, 2023, 06:37

Hello everyone,

I did not read all the threads. But I have done sth about calculating the yPlus value for all cells. I modified the code of chegdan for calculating yPlus for all cells. Thanks for his contribution.
This is the link to the old code: https://github.com/chegdan/yPlusUplus.
This is the link to my code: https://github.com/Ruansh233/RshOpen.../main/yPlusCFD

The old version is run on OF-2.1. And my new version can run on OF-v2106
I delete some redundant steps and omit to create too many new objects. My code is running much faster compared to the old version.

March 14, 2015, 10:21	plusPostRANS	#108
hamsteri15 New Member Petteri Join Date: Feb 2014 Posts: 11 Rep Power: 12	I have a question about the plusPostRANS utility. If I understood correctly, the average(uTauWall) function calculates the wall-average of u_tau. So for a flat plate flow ,for example, if I wanted to plot the dimensionless velocity profile at certain x-coordinate location using the u+ and y+ values output from the utility, the values are actually quite far off? Has anyone come up with a nice way to plot the accurate dimensionless velocity profile with low-Re models? So far I've always calculated the u+ and y+ manually using the velocity gradient (wallGradU) at certain point but for more complex geometries this is quite tedious. Is it possible to modify the utility so that it uses the same location for the surface normal gradient of the velocity and the point at the wall it calculates the distance to?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Low values of Lift force	vmlxb6	CFX	1	February 2, 2011 06:13
Incompressible Turbulence models	achinta	OpenFOAM	4	May 27, 2010 11:35
turbulence models?	haider	FLUENT	0	March 8, 2006 00:58
Turbulence Models and external flow.	Alan	FLUENT	3	November 22, 2005 05:46
Turbulence boundary values	lego	CFX	9	October 25, 2002 12:55

May 11, 2014, 08:13		#101
HanSolo123 New Member Hans Barósz Join Date: May 2014 Posts: 22 Rep Power: 12	Hello, I have the same problem like aylalisa. The post-Processing utility "wallShearStress" actually only works for RANS-Simulation. I actually dont understand why it is so but ok. I found a thread here on the forum how to calculate the wall shear stress tau_w for LES( http://www.cfd-online.com/Forums/ope...imulation.html ) but this does not work for OP2.3.0 anymore. I had a look in wallShearStress.C, but there is no reference to #include "incompressible/RAS/RASModel/RASModel.H" anymore as mentioned in the above thread. I want to plot u+ over y+ as well, therefor I need u+. When I extract u_tau from y+, is it possible to calculate u+ then with u+ = u / u_tau? I am unsure about the directions. In which direction points u_tau, when you have a simple Channel flow in x-direction? When I extract it from y+, does it point in x-direction then? The u+ over y+ graph is actually a dimensionless velocity profile, so it is velocity in x over wall distance in y. But i am unsure about u_tau. Any tips?

May 4, 2018, 10:09		#113
wouter Senior Member Wouter van der Meer Join Date: May 2009 Location: Elahuizen, Netherlands Posts: 203 Rep Power: 18	Hello gu1, The utility was written for OF2.3.x. So compiling for OF3.0 can give problems. I cannot help you solve it, but you can download OF2.3.x and use that to run your model and the utility or you can find out what changed between OF2.3 and OF3.0 and adapt the utility to OF3.0 (please post the adapted utility if you do). Best regards, Wouter

June 25, 2019, 01:58		#114
calf.Z Senior Member Jianrui Zeng Join Date: May 2018 Location: China Posts: 157 Rep Power: 8	how can I plot y+ and u+ in OpenFOAM. Dose anyone modify the tools? Thank you.

August 23, 2023, 06:37		#115
fly_light New Member Shenhui Ruan Join Date: Nov 2021 Location: Karlsruhe Posts: 16 Rep Power: 4	Hello everyone, I did not read all the threads. But I have done sth about calculating the yPlus value for all cells. I modified the code of chegdan for calculating yPlus for all cells. Thanks for his contribution. This is the link to the old code: https://github.com/chegdan/yPlusUplus. This is the link to my code: https://github.com/Ruansh233/RshOpen.../main/yPlusCFD The old version is run on OF-2.1. And my new version can run on OF-v2106 I delete some redundant steps and omit to create too many new objects. My code is running much faster compared to the old version.