Hello All!

I'm trying to get this simulation to converge quicker, and since each attempt takes a day to test I thought I'd see if there was some guru advice that could speed my progress...

I am simulating a hull moving through water. The hull 18m long x 5m wide, and about 0.6m deep under water (keel 3.7m), 2m high over water. The rectangular domain is 30m wide, 50m long and 10+5m deep/high.

This image gives you an idea of what it looks like:



The properties of interest are the force_xyz() and torque_xyz() on the hull body.

The mesh is approx 1.7M elements. The hull boundary layer prism mesh is 25 layers deep, first layer 0.02 mm thick and then growing exponentially with a 1.25 factor. This gives me a y+ value of around 4-6 at the leading edges, while still beeing deep enough to contain most of the boundary layer at the trailing. Surface mesh on the hull is Quad dominant, sizes from 50mm to 10mm depending on level of detail, finer at critical areas such as airfoil edges. The mesh is fairly rough (1m) at the farfield.

An image just to convey an idea of the mesh:



I am using the following settings: - static multiphase boyant flow - Multiphase options: homogenous model, standard free surface model, interface compression = 2 - Heat Transfer: Homogenous, Option = None - Turbulence Model: SST, default settings, Bouyance Turbulence = 0. - Auto Timestep (1.33 s)

Inlet at the front is normal speed = 5 m/s, low intensity turbulence, volume fractions controlled by step function at the surface.

Outlet is Static Pressure with pressure function as per CFX Modelling Manual p192.

Running on a Windows XP 32bit dual processor system.

This is what a monitor of force_x() @ the hull body looks like:



A rough estimate of the correct hull drag (using the Delft Systematic Series II method) is 6.7kN, so we are in the right neighbourhood, but not exactly stable...

What I'm looking for is advice on how to improve/speed up convergence, since I'm going to be running a lot of different cases with this configuration.

- Change any model parameters? - Finer mesh? (I am close to the 2GB memory allocation limit of the solver) - Upgrade to 64bit?

Or maybe it's just supposed to run about like this and I need to go say 300 iterations or so ;-) ?

/C

Hi,

your outlet looks a little close. I would suggest 5 hull lengths. The problem with the outlet boundary condition ie. specifying a hydrostatic pressure distribution is that it is a bit wrong since the real flow will have a wake which persists for many hull lengths. This will cause a slight disturbance at the outlet and reflect back into the domain.

If you get farther away from the hull the deviation between hydrostatic pressure and the actual pressure in the wake lessens.

This effect is worse at low Fr numbers...in my experience.

Give it a try and let us know what you find.

Regards,

Bak_Flow

Hi,

Also consider the transitional turbulence model. The flow will probably have significant areas of both laminar and turbulent boundary layers so you need to account for that. This of course now means you need a grid with y+ of about 1 and there's no way you will run that on a dual CPU 32 bit machine. You will need to go parallel. 64 bit won't help unless you have a 64 bit machine with heaps of memory.

Glenn Horrocks

Will that depend on the boat speed? If boat speed is high enough, BL could be turbulent everywhere. Chebeba mentioned that the calculated drag force is about the right magnitude. I wouldn't try a fancy model if not necessary.

Is there any literature showing that SST model predicts flow badly if Y+>>1? I seldom drop the max Y+ value below 35 as it will cost millions of extra nodes to do that in my cases.

The other problem is that you seem to assume the model fixed in height. This should be fine if you are trying to compare Ranse results to towing tank data. But if sinkage is fixed (Delft are not) you will probably not get the expected resistance. Obviously solving the Ranse + body motions (sinkage + trim in this case) will prove very costly.

You are correct in the above. What I figure I will do is solve for sinkage "manually". What I mean is I will move the hull around for each case until I get the right bouyancy force.

The purpose of the simulation is to determine the hull CLR, which in turn determines mast placement.

/C

I am slightly bewildered by this too. I am not a turbulence model expert by any means. SST was the choice because it seems to be the most widely used and trusted model. The CFX docs says "you need at least 10 nodes in the boundary layer", but does not go on to define what they consider to be the boundary layer here.

Also the docs mentions an y+ limit of 11.06 where the solver switches wall model, which is why I kept my y+ at around 5.

It would be interesting to hear if anyone has more substance on this... /C

Hmm... The above comment was Re: TB's post above. Should have quoted the question I suppose, this forum does not illustrate the threads all that well

A simple way to speed up the results would be to change to a k-eps or k-omega model. Most of the ship free surface runs are have been done with such models, and have been found to give sensible results. These turbulence model will be faster, and you ll be able to go to higher values of y+ (50 in cfx should be fine). And you need several runs to get the required sinkage, + some leeway angles + some speeds, to get a good overview of the clr changes. So faster results (still reliable) are probably the way to go.

Hi,

Yes, the amount of laminar and turbulent flow will depend on the speed of the boat. Also the approach you take will also depend on whether you just need the lift/trim results of whether you want drag as well; and then how accurately you want drag.

It is likely you can use fully turbulent flow with y+ around the 20-40 mark to give reasonable lift and trim data. You will get a drag number from this but it's accuracy will depend on whether significant laminar flow regions occur at the leading edges.

Also if significant separation occurs then accurate results are more tricky again, but I am assuming the flow is attached.

From some of your previous posts it seems you are only trying to get the keel/rudder/hull lift, and fully turbulent flow with Y+ between 20-40 should be OK for that. You will probably find the SST turbulence model the best model for this type of application.

Glenn Horrocks

Regards, Glenn Horrocks

When ypu mean heaps of memory, what are those values of memory?

regards Dan

Well, I find that I can just about exactly fit my 1.9 M elements simulation on a 4GB machine at 64 bits. 32 bits needs about 2.5GB.

That's one datapoint, anyway.

By the way I am not seeing any significant difference in results between 32 and 64 bits on this particular problem. /C

Just posting a little reply to my own question in case someone else comes along with similar problems. Some conclusions from the last 10 days are:

1. Timestep settings should be approx an order of magnitude smaller for the volume fraction equations than for others. This gets rid of the rapid oscillations seen in my original post.

2. If the mesh is not fine enough to accuratly resolve the free surface, waves will form in the domain and cause longer (slower) oscillations. Thus convergence can actually be made a lot quicker by *increasing* mesh density. As an exampe I doubled the number of elements in my mesh, and went from maybe 200 to 50 iterations required for convergence, meaning even if calculation time per iteration doubled, total simulation time was still much lower.

3. Too small a domain will also cause waves and slower convergence.

4. Inlet turbulence can be set even lower than the "low" menu item (using Intensity/Lengh Scale option).

...and I'm shure there are other things as well!!

/C

[matled]

Hi,
just a question regarding the settings of the simulation. I can't find on the manual a description of the "interface compression" parameter. DOes anyone know something about it?

Thanks in advance