Here's a picture of a strange
 

Here's a picture of a strange behaviour at the surface of a water turbine runner, when using LienCubicKE and NonlinearKEShih in OF-1.4. The surfaces are colored by the turbulent kinetic energy, and everything that is not blue is incorrect. It looks like those colors should belong to some other variable. The behaviour does not appear when using the kEpsilon and RNGkEpsilon models.

I was first thinking that this might be post-processing, but since it appears both in Ensight and in paraFoam there is a risk that this actually affects the solution. The solution yields flow features that I can't explain physically, but they probably origin from this strange behaviour.

I also had a look at the domain decomposition for the parallel simulations, but there is no processor interface exactly in this position.

Did anyone see anything like this before?

http://www.cfd-online.com/OpenFOAM_D...ges/1/5503.jpg

Håkan

as i posted some weeks ago, i
 

as i posted some weeks ago, i had something similar.
i run a turbulent channel flow (normal one and also one with wall suction and blowing). with the nonlinear models ( i tried both with wall functions and lowre) the turbulent kinetic energy and the dissipation were always at one wall. first of all the kinetic energy should be zero at the walls and second in the normal channel flow the behaviour should be axissymetric. nobody could help me with that. i tried everything like playing with relaxation parameters and using the rng k-epsilon field as initial condition etc. how is your velocity field. does it give correct results?

Looking at circumferentially a
 

Looking at circumferentially averaged velocity profiles below the runner, the velocity actually looks fine. But then they are circumferentially averaged, and I expect that there is a difference in different positions in the circumference.

Looking at a pressure iso-surface there is a strange behaviour that might have its origin in the previously mentioned problem. In the following picture there is a non-axisymmetric (and non-periodic) pressure distribution at the runner cone. I am actually looking for this kind of structure, but the problem is that its location is steady in time (in the rotating coordinate system), which it shouldn't be. I also see that the pressure is not periodic on the five blades, so there will be a net force on the runner which there shouldn't be. This non-axisymmetric pressure at the blades is also steady in time in the rotating coordinate system.

http://www.cfd-online.com/OpenFOAM_D...ges/1/5505.jpg

Håkan.

the problem looks similar to m
 

the problem looks similar to mine. i also had problems with the pressure distribution. what are your boundary conditions for inlet outlet? and do you start the simulation with a converged rng-k-epsilon solution as initial condition?

The simulations are started fr
 

The simulations are started from a converged kEpsilon solution.

Boundary conditions:

U:
INLE (specified inlet b.c., looks good)
{
type fixedValue;
value nonuniform List<vector>
OUTL
{
type zeroGradient;
}
WALL
{
type fixedValue;
value uniform (0 0 0);
}
ROTI (some rotating walls)
{
type fixedValue;
value nonuniform List<vector>
ROTW (some rotating walls)
{
type fixedValue;
value nonuniform List<vector>

p:
INLE
{
type zeroGradient;
}
OUTL
{
type zeroGradient;
}
WALL
{
type zeroGradient;
}
ROTI
{
type zeroGradient;
}
ROTW
{
type zeroGradient;
}

k:
INLE (specified inlet b.c., looks good)
{
type fixedValue;
value nonuniform List<scalar>
OUTL
{
type zeroGradient;
}
WALL
{
type zeroGradient;
}
ROTI
{
type zeroGradient;
}
ROTW
{
type zeroGradient;
}

epsilon:
INLE (specified inlet b.c., looks good)
{
type fixedValue;
value nonuniform List<scalar>
OUTL
{
type zeroGradient;
}
WALL
{
type zeroGradient;
}
ROTI
{
type zeroGradient;
}
ROTW
{
type zeroGradient;
}

Håkan.

Have you recompiled using the
 

Have you recompiled using the bug fix for "TensorI.H" ?
"Tensor bug fix"

This might explain the differening behavior with the linear k-eps models (kEps, RNGkeps,..) which calculate the turbulent production, G, from the square of strain magnitude,

G = 2 * nu_t * magSqr( grad(U) )

as compared to the nonlinear models which calculate the production from a contraction ("&&" operator) of the velocity gradient and the turbulent stress,

G = stress && grad(U)

oh wow thanks for that hint. a
 

oh wow thanks for that hint. actually what does recompüile means? do i only have to overwrite that certain file on my hardrive or also something else?

and also is that patch working
 

and also is that patch working as well for openfoam 1.4?

The bug also applies to openfo
 

The bug also applies to openfoam 1.4 and I don't think "TensorI.H" changed between 1.4 and 1.4.1.
(you might check this before doing a replace)

By recompile, I meant to replace (edit) the existing "TensorI.H" with the posted version and recompile your OpenFOAM library.

Dave

should i recompile the whole s
 

should i recompile the whole src and applications or only src?

is that the right command?

foam
cd src
./Allwmake
cd ../applications
./Allwmake

I did not include this bug fix
 

I did not include this bug fix in these simulations. That is actually the kind of bug I expected to be the reason for this behaviour.

I hope that I will have the time to test the bug fix soon.

Thank you Dave!

Håkan.

Robert, You only need to re
 

Robert,

You only need to recompile from the first wmake you find in your tree: OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM
so, after you changed the TensorI.H, go there and wmake there
this is C++ power :o)

regards,
Cedric

when do the wmake i always get
 

when do the wmake i always get an error message like that:

maduta@linux-hiwi1:~/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM> wmake
make: Warning: File `Make/linuxGcc4DPOpt/dontIncludeDeps' has modification time 10 s in the future
make: Warnung: Mit der Uhr stimmt etwas nicht.
Die Bearbeitung könnte unvollständig sein.
SOURCE=OSspecific/Unix/signals/sigFpe.C ; g++ -m32 -Dlinux -DDP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -DWM_PROJECT_VERSION='"'1.4'"' -I/home/maduta/OpenFOAM/OpenFOAM-1.4/src/zlib-1.2.1 -IlnInclude -I. -I/home/maduta/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM/lnInclude -fPIC -pthread -c $SOURCE -o Make/linuxGcc4DPOpt/sigFpe.o
/bin/sh: g++: command not found
make: *** [Make/linuxGcc4DPOpt/sigFpe.o] Fehler 127
maduta@linux-hiwi1:~/OpenFOAM/OpenFOAM-1.4/src/OpenFOAM>


what could that be?

hi i managed to overwrite the
 

hi i managed to overwrite the TensorI.H file in the Tensor directory.
what i did then is going with the terminal to the /src/OpenFOAM directory and i made the command:
wmake /OpenFOAM/OpenFOAM-1.4.1/src/OpenFOAM/primitives/Tensor/TensorI.H

after making all the dependencies at the end i get an error like this:
finished, there are no rules to create TensorI.H

someone knows if that could be a compilation error due to ubuntu which i am using because suse didnt work.
or is there any mistake in my commands?
and also does this wrong tensor definition also affect the rsm-models? i guess so cause they also give me wronmg results

it would be nice if someone could help me :-)

Hi Robert! You have to rema
 

Hi Robert!

You have to remake the libOpenFOAM.so:

cd $FOAM_SRC/OpenFOAM
wmake libso

Bernhard

i just want to give an update:
 

i just want to give an update:
i finally managed to do a wmake libso in ubuntu with the new TensorI.H file. it all went well but the nonlinear models are still giving wrong results for channel flow, like totally non symmetric. so Håkan Nilsson if you find out something new plz let me know.

Hi all!

It's been a while since you wrote here but did someone find out what is wrong with the nonlinear models? I am also trying to use them, first some tests with a boundary layer flow. The results are different from the analytical solution and I thought maybe because from the original Shih paper mentioned in the code the dirac terms, i.e. the double dot products or the gradU are not implemented.

Did someone have the same feeling when comparing with the paper?

Aniko

generation term
 

Is there anyone who knows correct generation term for nonlinear turbulence model?

In all the nonlinear models in OpenFoam, the generation term looks like
G = nu_t * symm(grad(U)) && grad(U) - nonlinear_term (1)

I think the first term of G must be same as one in linear models.
In linear models such as kEpsilon,
G = nu_t * 2 * symm(grad(U)) && grad(U) (2)
= nu_t * 2 * magSqr(symm(gradU))

I can't understand why factor 2 is omitted in eq. (1).

If you know the reason or the correct generation for nonlinear turbulence model, please give your help to me.

Many thanks

Courant number increases
 

Hi all,
When run with the Cubic non-linear model Lien with the linear wall Function Courant number increases sharply and so soloution of problem is stops.:(
but when run with Nonlinear wall function I haven't this problem.
Please friends help me that how to solve this problem.
Thanks.

Hi jkim,
I agree with you , Because I work with nonlinear models for example quadratic Shih .
when that me use the first term of G (nu_t * symm(grad(U)) && grad(U)) result of solution
is uncorrect .
I run same model with G = nu_t * 2 * symm(grad(U)) && grad(U)- nonlinear_term that result is very good.
so, I think this approach is correct.

I am agree with you
 

************************************************** *
Hi jkim,
I agree with you , Because I work with nonlinear models for example quadratic Shih .
when that me use the first term of G (nu_t * symm(grad(U)) && grad(U)) result of solution
is uncorrect .:(
But , I run same model with G = nu_t * 2 * symm(grad(U)) && grad(U)- nonlinear_term that result is very good.:)
so, I think your opinion is correct.