Fluent parameters for sailing yacht analysis

[D_Mylonas]

Hello,

I am looking at the CFD analysis of an America´s Cup yacht in Gambit and Fluent and I was wondering if any of you can advise me on the parameters and boundary conditions one might use to obtain proper results.

I am concentrating on the hull and the appendages and plan to look for upright and heel condition (10-15-20-25 degrees). I do not take into account the geometry above the free-surface (waterline) and from the Gambit model, I have some initial conditions like wall surfaces for the yacht and the appendages, inlet velocity at inlet, outflow/pressure outlet at outlet, symmetry at centreline (for upright condition).

Any advice on turbulence modelling, advection scheme etc... would be very welcome!

Thank you for your help,

Dimo

[Tim B]

Is this a project, or a point of interest?

I have done a similar case in OpenFOAM (for a 35' Cruiser/Racer) and it is not as easy as it looks.

Run some simple cases first, just to get the right boundary conditions. I can't say exactly what they are, but take an educated guess then find the ones that don't let fluid drain out of the domain.

Now, for an upright case with no leeway I was using 1.5Million cells and a symmetry boundary on the centreline of the hull. If you want to get good answers, think in the region of 3 million cells per half-hull, or 6million at a heel/yaw condition.

This is some serious computing. You will need several computers and a lot of patience. I would advise that you pick your cases carefully.

Get in touch with Nico (on these forums), he'll be able to help, and I'm starting a job in Glasgow in July, so I'll be around then.

Good Luck,

Tim B.

[D_Mylonas]

Originally Posted by Tim B

Is this a project, or a point of interest?

I have done a similar case in OpenFOAM (for a 35' Cruiser/Racer) and it is not as easy as it looks.

Get in touch with Nico (on these forums), he'll be able to help, and I'm starting a job in Glasgow in July, so I'll be around then.

Good Luck,

Tim B.

Hi Tim and thank you for your kind help.

It's a bit of both actually! It's both part of a project and for my own interest. It all started last year when I was in my final year of university and our MEng project was on America's Cup yacht design and analysis. I was involved in CFD and I tried at the time to mesh the appendages and analyse the forces etc...with CFD. Unfortunately, there was no Nico at the time, and there was certainly no help or support from my supervisors and my superiors here in the department, therefore the attempt was aborted very quickly. Fortunately enough, we did some tank testing from which we got the results we wanted, but obviously CFD would have added something more to our project.

But I've continued and I'm now a PhD student and I am helping a 4th year student with his individual project, who tool from where we left and who now wants to use CFD to predict resistance of appendages of the AC yacht we designed and compare them with the tank testing we did. So I'm here helping him, and in the same time developing my own interest for the subject as my background is from yacht design/small craft and I'm sure will be useful for my future.

Now I've been using Gridgen rather than Gambit, and so far I managed to tackle separately the bulb and the keel and now I'm the process of meshing them both. The cell numbers you mention are in the range of my grid generation, and indeed running this on several computers will be necessary. Because time is running out we'll focus mainly on Upright condition with no leeway and after on heeling with no yaw.

I'm lucky enough to be sitting two desks behind Nico, and he's been helping us with the work to be done. We use half the geometry with centreline as symmetry, the hull and appendages as non slip wall, the inlet as velocity inlet, outlet as pressure outlet, top, bottom as walls and farfield as wall or farfield. For turbulence we'll try realizable k-eps model, with default values, unsteady flow, VOF for free-surface condition (i.e hull and heeling condition at angles 20-25 deg).

Hopefully we'll be able to get some results, otherwise I was thinking of scaling the model down to the size of the model used in the tank testings and then using similarities laws to scale the results to full size and compare with our results from last year. But then there might be some discrepencies between Froude and Reynolds numbers when scaling. But it is indeed hard and as you mentioned it needs a lot of patience

Anyway thank you for your advices, if you have anything more to add you are very welcome, otherwise it'll be nice to discuss of the problem in July, although the project finishes in May. If you come with more suggestions, please do not hesitate to post them

[nico]

(having spent a bit of time on looking for things that work, this might be of interest to several of you).
1) at inlet: velocity inlet: velocity and phase are prescribed (phase using UDFs).
2) at outlet: pressure outlet: hydrostatic pressure and backflow phase are prescribed (both using UDFs).
3) since hydrostatic pressure is modeled (a body force), the pressure interpolation needs to be Presto! or Body force weighted.
4) typical time steps are around 0.006s.
5) total simulated time is around 7s.


The UDFs follows: (two functions, assumes free surface at z=0.0)

/*
  DEFINES PHASES CONCENTRATION
*/
DEFINE_PROFILE(phase2_inlet, thread, position)
{
  real x[ND_ND];		/* this will hold the position vector */
  real z;
  face_t f;
  begin_f_loop(f, thread)
    {
      F_CENTROID(x,f,thread);
      z = x[2];
      if(z>=0.0){F_PROFILE(f, thread, position)=0;}
      if(z<0.0){F_PROFILE(f, thread, position)=1;}
    }
  end_f_loop(f, thread)
}


DEFINE_PROFILE(outlet_p, thread, nv)
{
	face_t f;
	real x[ND_ND];
	begin_f_loop(f,thread)
	{
	F_CENTROID(x,f,thread);
	if(x[2]>=0.0)
	F_PROFILE(f,thread,nv) =0.0;
	else
	F_PROFILE(f,thread,nv) =998.2*9.81*(0.0-x[2]);
	}
	end_f_loop(f,thread)
}

Concerning Dimo's problem, I would definitely compare results at model scale. (mesh would actually be easier to model, and computing time will be lower).

[D_Mylonas]

Originally Posted by nico

Concerning Dimo's problem, I would definitely compare results at model scale. (mesh would actually be easier to model, and computing time will be lower).

Thanks for the tips Nico, they are truly invaluable bearing in mind the time left for this project.

However I doubt that Dani used the scaled model for a start, which might be one of the reasons why he's getting so much problems meshing the full scale hull in Gambit. I shall advise him to try at model scale, and I shall do it also for the appendages, although so far so good with a full-scale bulb and Gridgen.

When free-surface is not intervening, I guess the parameters are different or simplified (i.e. no VOF, hydrostatic pressure simplified)?

Dimo