Aah, my mistake. I was wonderi
 

Aah, my mistake. I was wondering where g was hiding.

Still, the pressure does behave strangely toward the bottom of the outlet and the removal of gravity makes the problem as described above go away. I will have another look at the formulation when I have some time.

Belay that, after a second loo
 

Belay that, after a second look I dont believe there is anything wrong at or near the outlet.

Dear Mattijs, thanks for the
 

Dear Mattijs,
thanks for the help. I tried to compile the new zipUpMesh, but I experienced problems (the compilation of the old zipUpMesh executable was instead straightforward).
I obtained the following errors after issuing wmake:
Making dependency list for source file zipUpCells.C
Making dependency list for source file zipUpMesh.C

SOURCE_DIR=.
SOURCE=zipUpCells.C ; g++ -m64 -DlinuxAMD64 -Wall -W -Wno-unused-parameter -march=opteron -O3 -ffast-math -fno-gcse -DNoRepository -ftemplate-depth-30 -I/home/michele/OpenFOAM/OpenFOAM-1.1/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -c $SOURCE -o Make/linuxAMD64Opt/zipUpCells.o
zipUpCells.C: In member function `void Foam::polyMesh::zipUpCells()':
zipUpCells.C:134: error: `WarningIn' undeclared (first use this function)
zipUpCells.C:134: error: (Each undeclared identifier is reported only once for each function it appears in.)
make: *** [Make/linuxAMD64Opt/zipUpCells.o] Error 1

However, if you are interested on a test mesh, the following link is that of the case under discussion:
www.lem3.it/tests/waves_050601/waves.tar.gz

Michele.
PS. Henry, I've just started a simulation with low order approximations, walls whose condition was set to 2 m/s (in rasInterFoam is not coded the slipWall condition, am I right?), and compression coefficient for gamma of 1.0. I will obtain results in about 3 hours...

Hi Michele, Sorry, didn't t
 

Hi Michele,

Sorry, didn't try it under 1.1.

Replace in zupUpCells.C

WarningIn("XXXX")

with

Warning<< "XXXX"

Hi Mattijs, thank you. Now
 

Hi Mattijs,
thank you.
Now the utility zipUpMesh works correctly. The corrected mesh passes all the tests of the checkMesh.

Thanks,
Michele.

Dear Henry: >> Why do you t
 

Dear Henry:

>> Why do you think there is a problem with the oulet pressure BC? Remember we are solving for pd which is p - rho*g*h, i.e. is constant with depth at the outlet.

Excuse me, Henry, isn't pd = p - g*h ?
I expect for pd the dimensions [m^2/s^2], am I correct?
Another question about the pressure. I'm interested in computing the pressure around floating bodies (and integrate pressure and viscous/turbulent stress over surfaces in order to obtain overall forces).
It is rather complicated to obtain pressure: if I use the expression p = pd + gh, h is not a constant as it depends on the wave elevation above each point.
That is to say that
p = pd + int(-gamma*g, ds)
an integral to be computed along the g direction (gamma is zero in air and one in water, introduced in order to capture the surface).
But below a floating body it is impossible to integrate up to a free surface (this space is occupied by the floating body itself!).
Have you any suggestion?

Ragarding the simulation, I'm making the run with the parameters you suggested.
However my impression is the following: it seems to me that boundary conditions don't pose any problem on the solution: all the instability grows well after the flow enters the domain. It resembles more a turbulence generated instability...
By the way, I would like to get the eddy viscosity among the output results... is it automatically possible or does this require coding?

> Excuse me, Henry, isn't pd =
 

> Excuse me, Henry, isn't pd = p - g*h ?

No pd = p - rho*(g.h) and you can calculate p from pd using this expression. Notice the dimension of pd:

dimensions [1 -1 -2 0 0 0 0];

h is the the position vectors of the cell centres and g is the gavitational force vector.

You can get the eddy viscosity from the turbulence model and write it out.

Hello, I also have a simila
 

Hello,

I also have a similar problem at the inlet of my 3d domain. As shown in the following pictures (with isosurface at gamma=0.5) (t=0.03), soon after the start of the computation, a 'wave' is developing near the inlet, and gets bigger and bigger.

meshCheck is ok.

my boundaries
pd:
boundaryField
{
inlet
{
type zeroGradient;
}

inlet:002
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

bottom
{
type zeroGradient;
}

top
{
type totalPressure;
p0 uniform 0;
value uniform 0;
}


right
{
type zeroGradient;
}
hull
{
type zeroGradient;
}
sym
{
type zeroGradient;
}
}

U:
boundaryField
{
inlet
{
type fixedValue;
value uniform (0.5 0 0);
}
inlet:002
{
type fixedValue;
value uniform (2 0 0);
}
outlet
{
type zeroGradient;
}
top
{
type pressureInletOutletVelocity;
phi phi;
rho rho;
value uniform (0 0 0);
}
bottom
{
type fixedValue;
value uniform (0 0 0);
}
sym
{
type fixedValue;
value uniform (0 0 0);
}
right
{
type fixedValue;
value uniform (0 0 0);
}
hull
{
type fixedValue;
value uniform (0 0 0);
}
}

http://www.cfd-online.com/OpenFOAM_D...ges/1/2101.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/2103.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/2102.jpg

As I said before, OF is not re
 

As I said before, OF is not ready for open channel yet. At least the inlet and outlet boundary conditions will cause problem.

Hi liu,nicolas i did numeri
 

Hi liu,nicolas

i did numerical simulations of a 2d hydrofoil in a channel. my preliminary results are 100% ok. i also had issues with the correct BC. but the VOF works for open channel flows. nicolas , please see my posts rasInterFoam - STRANGE RESULTS AT BOUNDARY . after i incorporated Hrv's suggestions my simulations went smooth

regards

kumar

Hi, kumar, Which post are you
 

Hi, kumar,
Which post are you refering to? I can't find it. Can you upload your case? I am so interested to see where I did wrong.

Thank you.

It's here http://www.cfd-onli
 

It's here
http://www.cfd-online.com/cgi-bin/Op...show.cgi?1/656

oops, actually it s this one
 

oops, actually it s this one

http://www.cfd-online.com/OpenFOAM_D...es/1/2014.html

I have checked the thread, but
 

I have checked the thread, but i do something similar in my case. My problem is at the inlet and not at the outlet.

Can anyone supply or point me
 

Can anyone supply or point me toward an implementation of outlet boundary conditions for free surface wave transmission?

Hallo, I have the following
 

Hallo,
I have the following problem: I have a solid surrounded by air that moves from the left to the right with a constant velocity. However I get a very high pressure wave on the interface solid-air at the inlet and at the outlet. I have the feeling, that something with the boundary conditions is wrong. Can anybody give me a hit what the problem could be?
Regards,
Karl-Heinz
P.S. I would like to add a picture of my problem. Can anybody tell me how to do that?

Hallo, concerning my problem
 

Hallo,
concerning my problem with the strange pressure patterns on the interface solid air. Here is a picture of my current model.
http://www.cfd-online.com/OpenFOAM_D...ges/1/5878.jpg
I use a modified interFoam solver. However these pressure waves make my silulation unstable.
Best regards,
Karl-Heinz

Hi all, I'm dealing with surface problems in interFoam, the post is:

http://www.cfd-online.com/Forums/ope...-sloshing.html

Any comments are welcome. Regards.

VOF Method
 

Dear All

Could I ask you whether you could tell me which VOF technique is used in OpenFOAM? I mean there are different VOF models like Hirt and Nicols, Youngs, and so on. Which one is used in OpenFOAM?

Regards
Ehsan

Dear ehsan
1) please ask your question just in one post, not in several posts!
2) look this paper:
this method reduces need for interface reconstruction, this method interface is smeared among 2 or 3 cells and it uses a high order schemes
and interface compression method to keep interface sharp
3) if you uses interFoam solver look at here:
4)if you look for more, look at here: