[mks]

Hello, Redondo

i've just starded calculating the case in OF1.6. I had to change all 'pd' in 'p' and all 'gamma' in 'alpha1' (in fvSchemes change 'gamma' to 'alpha'). Don't forget to rename the files in 0 dir accordingly (p und alpha1)

That seems to work

[g.redondo]

Thanks mks,

I forgot to post how I did it, but the problem is already solved pretty much doing what you mentioned. The only thing I'm missing is how to separate hydrodynamic and aerodynamic forces. Any clue?

Gonzalo

[g.redondo]

Hi all,

I wonder how are you doing with OF1.6 for free surface flows. I was able to run robust simulations, but the forces are way off the experimental data, about twice:

Pressure Forces:
Fpx = -0.212253, Fpy = 0, Fpz = 25.228174

Viscous Forces:
Fvx = -0.427812, Fvy = 0, Fvz = 0.045150

I don't bother too much about viscous forces at this stage but what is killing me is that I cannot figure out what is going on with pressure forces.

Here I'm showing the results for a 514K mesh with at T=10 seconds. Timestep is 0.002s and turbulence model is kOmegaSST. There's a 0.7 relaxation on p. Anyway, if somebody has a clue about the issue with the forces or just want some help I can post or attach some files

Turbulence off does not solve pressure forces, it's all pretty much the same. I also tried other turbulence models and different yPlus. Right now it is around 100.

wigley_540_ISO_Zcontours_10s.jpg

wigley_514_VOF_10s.png

[jploz]

Hello,

how do you calculate the forces? I've done comparison calculations using Wigley hulls and containerships which showed good agreement with experimental data. The forces were calculated using a modified functionObject 'forces' since the original one does not support two phase flow.

HTH,
Jean-Peer.

[g.redondo]

Hi Jean-Peer,

You're correct about the original force function, but I also made a filter with paraview and the pressure forces are pretty much the same (neglecting aerodynamics). Would be nice to know about your modified function though.

I think that the problem I'm facing is new in OF1.6 as Eric has shown very nice results with previous versions. The case had to be ported and doesn't seem to work so nice, although as you can see free surface is not too bad.

Gonzalo

[jploz]

I've used both version 1.5 und 1.6 and the resulting forces were nearly the same. There were differences but not of factor 2! So, in principle it should be possible to use 1.6. My final investigations were conducted using the version 1.5-x and I think the use of the modified pressure is more appropriate within the current solver framework.

Did you apply a 'bouyantWallPressure' BC at the hull?

The modifications I did is to take the variable density and viscosity into account rather using a constant reference density. However, this does not impact the pressure force.

[g.redondo]

Thanks for the quick reply, I appreciated it. It is also good to know that it's working for you.

I'm using zerogradient for the pressure on the hull. Outlet is buoyantPressure. Should it also be buoyantPressure on the hull? How did you set up the boundaries?

I will try the modification of the force function after fixing this.

Gonzalo

[jploz]

Hello Gonzales,

IMO zeroGradient is not the proper BC for the hull in 1.6. You should use 'buoyantPressure 0' instead. As far as I understood, buoyantPressure is a fixed gradient BC that takes the impact of the buoyancy into account. Thus, the use of 'buoyantPressure 0' and zeroGradient is equally in the case of vertical wall but is not if the wall arbitrary located (as the hull) or is a horizontal wall (as the bottom).

Some comments on my BCs: the application of zeroGradient for the outlet did not work very well for me (especially in combination with unstructured grids), so I prescribed the pressure (profile) on the outlet. The inlet was modelled as velocity inlet and remaining bounds as free slip walls.

Good luck.
Jean-Peer

[g.redondo]

Ok, got it.

I will try with buoyantPressure at the hull and I'll post the results here as soon as possible, if any

Gonzalo

[Schag]

hello,
I'm very interested in the results of buoyantPressure on the hull.
As Jean-Peer said, buoyantPressure has a "strange" impact on non vertical interface. You can see what I obtained in another topic
http://www.cfd-online.com/Forums/ope...interface.html
I didn't find an equivalent to zeroGradient in 1.5 for Pressure. If I put zeroGradient in 1.6, I don't have mass conservation.

Waiting for your opinion.

Regards

[g.redondo]

Hi all,

Still running, it is slightly less but not sure if enough. I will post results when (and if) it gets to 5s (this night here in Spain).

The only difference I think I have compared to Jean is that instead of having free-slip walls at the side and bottom I have it all defined as an inlet. The reason why I do this is to keep the same setup as CCM and Comet. I'm gonna try changing it by I don't think it's the problem.

I'm running a structured grid.

Here I paste my U:

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

internalField uniform (-0.9897 0 0);

boundaryField
{
OUTLET
{
type zeroGradient;
}
SYMMETRY
{
type symmetryPlane;
}
ATMOSPHERE
{
type pressureInletOutletVelocity;
value uniform (-0.9897 0 0);
}
EXTRAHULL
{
type zeroGradient;
}
INLET
{
type fixedValue;
value uniform (-0.9897 0 0);
}
HULL
{
type fixedValue;
value uniform (0 0 0);
}
}


and also my p file:



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

internalField nonuniform List<scalar>
286572
(
14192.7
12528.2
11062.6
9772.02
............
............
0.193104
0.123309
0.0429817
)
;

boundaryField
{
INLET
{
type buoyantPressure;
gradient uniform 0;
rho rho;
value nonuniform List<scalar>
17080
(
14192.7
14192.7
14192.7
............
............
0.193104
0.123309
0.0429817
)
;
}
EXTRAHULL
{
type buoyantPressure;
gradient uniform 0;
rho rho;
value uniform 0;
}
ATMOSPHERE
{
type totalPressure;
rho none;
psi none;
gamma 1;
p0 uniform 0;
value uniform 0;
}
OUTLET
{
type buoyantPressure;
gradient uniform 0;
rho rho;
value uniform 0;
}
SYMMETRY
{
type symmetryPlane;
}
HULL
{
type buoyantPressure;
gradient uniform 0;
rho rho;
value uniform 0;
}
}

[Ahmed]

This might help
http://www.iihr.uiowa.edu/~shiphydro...S60_steady.htm
http://gfs.sourceforge.net/examples/...ip.html#htoc11

Good Luck

[g.redondo]

Ok, thanks Ahmed.

According to Jean-Peer I run the simulation with buoyantPressure BC at the hull.

The resulting forces are the following:

Fpx = -0.162647
Fpz = 25.119922
Fvx = -0.567550
Fvz = 0.065198

So it is better in terms of pressure forces, I can't say the same about viscous though. Anyway, it looks like the way to go, but it is still far from the target of Fpx = -0.1232 and Fvx = 0.3577.

I was thinking on making a wider domain because of my sides(inlets). I will also run a simulation with free slip walls just to see the difference between both approaches.

This are the settings that I still have to investigate properly, what are you using?

- Domain Size (I think it's big enough, check it on the TOP view, but as I said I'll make it bigger just to try)

- Turbulence model (KOmegaSST, also tried KEpsilon)

- Yplus (50~100)

The mesh density didn't affect before (zeroGradient BC), so I don't that'll change with the buoyantPressure BC. Therefore I'm investigating on the coarse mesh (286K). Here I attach some pictures at 5s.

wigley_286_ISO_Zcontours_5s_small.jpg

wigley_286_Zcontours_5s_small.png

wigley_286_VOF_5s_small.png

[jploz]

Hello everybody,

As Jean-Peer said, buoyantPressure has a "strange" impact on non vertical interface.

To clarify: I don't think the buoyantPressure BC has any strange impact. In fact, it takes the gravity (and thus the resulting constant pressure gradient) into account and is the right BC for non-vertical walls when using the interFoam solvers in 1.6.

@g.redondo
Some more remarks:
1. I'm sure the grid resolution has impact on the computed resistance, in particular the pressure resistance. IMO, you cannot expect to get results that match exactly the experiments with somewhat 200K cells.

2. Did you investigate the time history of your forces. There are oscillations in the (pressure) forces that take time to vanish. Have a look at that and take a time average, maybe.

HTH,
Jean-Peer.

[Schag]

Originally Posted by jploz

Hello everybody,

To clarify: I don't think the buoyantPressure BC has any strange impact. In fact, it takes the gravity (and thus the resulting constant pressure gradient) into account and is the right BC for non-vertical walls when using the interFoam solvers in 1.6.

Ok, my mistake, I didn't get what you meant. Did you have a look at my topic? How can you explain the behaviour of water in my case?

Regards,

[g.redondo]

Originally Posted by jploz

@g.redondo
Some more remarks:
1. I'm sure the grid resolution has impact on the computed resistance, in particular the pressure resistance. IMO, you cannot expect to get results that match exactly the experiments with somewhat 200K cells.

I know, but I would expect it to be closer, as it is in CCM with the same mesh (Fpx ~ -0.013). I tried the same settings with a 286K, a 514K and a 915K mesh. All results are pretty much the same.

Originally Posted by jploz

@g.redondo
2. Did you investigate the time history of your forces. There are oscillations in the (pressure) forces that take time to vanish. Have a look at that and take a time average, maybe.

I did. The results I'm giving are an average of the last 500 timesteps.

In my opinion, there must be something else.

[g.redondo]

Hi all,

Still struggling with this. The following is my current situation after another week of investigations on this simulation.

These are the investigations I've done so far:

- Simulation time: I concluded that the simulation stabilizes at t=5s

- Mesh size independence investigation (286K, 514K and 914K): Results show no differences between them in terms of forces and free surface.

- Domain size investigation: With two step variations I've checked the length upstream, downstream and also the width. No differences.

- Turbulence model investigation (KEpsilon, KOmega and KOmegaSST): No differences.

- Yplus investigation (~30, ~100, ~200). The smaller it is the bigger the viscous forces are. Pressure remains the same.

Right now I'm still ~20% off in pressure forces and ~80% off in viscous. What could be the reason for so high viscous forces?

I wonder if someone has validated interfoam 1.6 with this case.

Best Regards,

Gonzalo

[egp]

Hi Gonzalo,

I've not used 1.6 extensively, but this is alarming given that you are taking a case from 1.5 and getting very different results.

In general, I do not like the idea of solving for total pressure. For the simplicity of initial and boundary conditions, I much prefer solving for the dynamic pressure and would be inclined to modify interFoam back to the 1.5 formulation. Also, the hydrostatic component tends to mask convergence problems due to the large amplitude in comparison to the delta between iterations. In one test with 1.6, my pressure forces looked strange, and upon subtraction of the hydrostatic component (in my post-processing tool), I could see that the dynamic component had lots of problems in regions of high grid clustering.

This of course doesn't explain the discrepancy in the viscous component. Since your mesh is a wall-function mesh, are you sure your b.c. are set correctly? 1.6 changed the wall-function implementation.

Eric

Originally Posted by g.redondo

Hi all,

Still struggling with this. The following is my current situation after another week of investigations on this simulation.

These are the investigations I've done so far:

- Simulation time: I concluded that the simulation stabilizes at t=5s

- Mesh size independence investigation (286K, 514K and 914K): Results show no differences between them in terms of forces and free surface.

- Domain size investigation: With two step variations I've checked the length upstream, downstream and also the width. No differences.

- Turbulence model investigation (KEpsilon, KOmega and KOmegaSST): No differences.

- Yplus investigation (~30, ~100, ~200). The smaller it is the bigger the viscous forces are. Pressure remains the same.

Right now I'm still ~20% off in pressure forces and ~80% off in viscous. What could be the reason for so high viscous forces?

I wonder if someone has validated interfoam 1.6 with this case.

Best Regards,

Gonzalo

[g.redondo]

Hi Eric,

I completely agree with you about masking dynamic pressure convergence.

You can check U and p in a previous post, but I think they're correct. K, Omega and nut are the same as for 1.5.

About that case you've run in 1.6... what results do you have for the viscous forces?

Soon I'll be running out of ideas so the last option would be to go back to 1.5, but only if I know that the old formulation is going to come back.

Regards,

Gonzalo

[matteoL]

Hello redondo,
I think that in OF-1.6 you have to set different BC for the turbulence terms.

mut for example should become (at least int the interfoam tutorials looks like this):

Wigley
{
type mutWallFunction;
value uniform 0;
}

and not zeroGradient as in 0F-1.5.

Is that what you have in your cases?

I agree with Eric about the dynamic pressure approach, in our cases it should be much better.

One question:
has anyone managed to have the 6-dof motion working in parallel with OF1.5-dev? I managed to have it running in serial, but in parallel I have same strange error like in the mesh motion solver (something I haven't touched at all): "operator T ()() temporary deallocated"..

I would just like to know if it is just my problem or if anyone has it working and thus I may have done something wrong.. (p.s: I have the blocking option)

Thanks,
Matteo