CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Strange behaviour when using LienCubicKE and NonlinearKEShih

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 27, 2007, 05:08
Default Here's a picture of a strange
  #1
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
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?



Håkan
hani is offline   Reply With Quote

Old   September 27, 2007, 05:24
Default as i posted some weeks ago, i
  #2
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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?
roberthino is offline   Reply With Quote

Old   September 27, 2007, 05:56
Default Looking at circumferentially a
  #3
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
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.



Håkan.
hani is offline   Reply With Quote

Old   September 27, 2007, 06:16
Default the problem looks similar to m
  #4
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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?
roberthino is offline   Reply With Quote

Old   September 27, 2007, 06:47
Default The simulations are started fr
  #5
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
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.
hani is offline   Reply With Quote

Old   September 27, 2007, 09:53
Default Have you recompiled using the
  #6
Member
 
E. David Huckaby
Join Date: Mar 2009
Posts: 57
Rep Power: 8
david_h is on a distinguished road
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)
david_h is offline   Reply With Quote

Old   September 27, 2007, 10:10
Default oh wow thanks for that hint. a
  #7
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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?
roberthino is offline   Reply With Quote

Old   September 27, 2007, 10:18
Default and also is that patch working
  #8
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
and also is that patch working as well for openfoam 1.4?
roberthino is offline   Reply With Quote

Old   September 27, 2007, 10:29
Default The bug also applies to openfo
  #9
Member
 
E. David Huckaby
Join Date: Mar 2009
Posts: 57
Rep Power: 8
david_h is on a distinguished road
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
david_h is offline   Reply With Quote

Old   September 27, 2007, 10:45
Default should i recompile the whole s
  #10
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
should i recompile the whole src and applications or only src?

is that the right command?

foam
cd src
./Allwmake
cd ../applications
./Allwmake
roberthino is offline   Reply With Quote

Old   September 27, 2007, 10:49
Default I did not include this bug fix
  #11
Senior Member
 
Håkan Nilsson
Join Date: Mar 2009
Location: Gothenburg, Sweden
Posts: 193
Rep Power: 8
hani is on a distinguished road
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.
hani is offline   Reply With Quote

Old   September 27, 2007, 10:53
Default Robert, You only need to re
  #12
Senior Member
 
Cedric DUPRAT
Join Date: Mar 2009
Location: Belgium
Posts: 179
Rep Power: 8
cedric_duprat is on a distinguished road
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
cedric_duprat is offline   Reply With Quote

Old   September 27, 2007, 12:24
Default when do the wmake i always get
  #13
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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?
roberthino is offline   Reply With Quote

Old   September 29, 2007, 06:53
Default hi i managed to overwrite the
  #14
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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 :-)
roberthino is offline   Reply With Quote

Old   October 1, 2007, 06:29
Default Hi Robert! You have to rema
  #15
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Robert!

You have to remake the libOpenFOAM.so:

cd $FOAM_SRC/OpenFOAM
wmake libso

Bernhard
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   October 1, 2007, 13:28
Default i just want to give an update:
  #16
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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.
roberthino is offline   Reply With Quote

Old   May 10, 2012, 11:02
Default
  #17
New Member
 
Aniko Rakai
Join Date: Oct 2009
Location: Budapest
Posts: 29
Rep Power: 7
ancsa is on a distinguished road
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
ancsa is offline   Reply With Quote

Old   January 30, 2013, 06:16
Question generation term
  #18
New Member
 
Jongtae Kim
Join Date: Mar 2009
Location: Daejeon, Republic of Korea (South)
Posts: 5
Rep Power: 8
jkim is on a distinguished road
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
jkim is offline   Reply With Quote

Old   March 6, 2013, 10:50
Default Courant number increases
  #19
New Member
 
Akbar Mohammadi Ahmar
Join Date: Oct 2012
Location: Tehran , Iran
Posts: 4
Rep Power: 4
akbarMohammadiAhmar is on a distinguished road
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.
akbarMohammadiAhmar is offline   Reply With Quote

Old   March 6, 2013, 11:01
Default
  #20
New Member
 
Akbar Mohammadi Ahmar
Join Date: Oct 2012
Location: Tehran , Iran
Posts: 4
Rep Power: 4
akbarMohammadiAhmar is on a distinguished road
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.
akbarMohammadiAhmar is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
IcoFoam strange behaviour when gravity is included nicasch OpenFOAM Running, Solving & CFD 5 August 29, 2014 10:09
buoyantFoam OF15 very strange behaviour in hotRoom andrea_barbera OpenFOAM Running, Solving & CFD 4 July 30, 2009 09:06
Strange multicomponent source behaviour Zitron CFX 4 July 12, 2007 15:32
Strange Behaviour in CFX-Mesh Kasper CFX 0 May 14, 2007 08:24
Strange behaviour in Coffus Luis Filipe Fabiani Phoenics 0 June 1, 2006 11:23


All times are GMT -4. The time now is 12:02.