[CFDKevin]

Greetings Foamers and boat enthusiasts!

The simulation of planing hulls has proved to be a challenging topic for many years. I wonder if anyone has found a good method for running these analysis with OpenFOAM. The main goals are usually to study sinkage, trim and drag. I know that this topic has been brought up before, but a general "good practice" method is lacking.

The obvious way to go about this is to start out with interFoam and run the case to steady state, then make the switch to interDyMFoam. The main challenge lies in stability, especially with interDyMFoam.

Without providing all details of my setup at this stage, I hope to start a discussion around the topic. If anyone has experience with simulation of boats, yachts or ships, please share. General know-how regarding interFoam or interDyMFoam is also very much appriciated!

[hjasak]

Hi,

My group at Uni Zagreb is running a project on added resistance in waves for large planning hulls. As a first step we did steady resistance (with sinkage and trim, obviosly).

We are using thd Naval Hydro pack with the wholg bag of tricks. The simulations run fine but we are stll learning about required meah resolution etc. Rhe forces on meahes of the order of 1.5 M cells are about 8% out, but I'm sure we will get better.

I think you have no chance with interFoam. It will ventilate, have a bad 6-dof solver (damping) and the interface jump conditions arent available.

Please send me an email if you'd like to hear more,

Hrv

[JNSN]

Hi Kevin,

simulations of planning hulls is definitely a challenging task for all CFD codes. Anyway, in my experience you can get very good results with interDyMFoam, and the 6DoF solver works absolutely fine for this.

I dont see the need to run interFoam in a first step. In order to ensure stability during start-up, you should ramp the forces. This option is available in the dev-Version:
https://github.com/OpenFOAM/OpenFOAM...7ec88e3cdb127a

For minimization of ventilation, a well designed mesh is necessary. Besides, there is an additional compression option together with an interfaceCompression-BC:
https://github.com/OpenFOAM/OpenFOAM...4ec11bb04bafb7

I have just done a small test with the new BC, and so far it looks quite promising.

Hope this helps,
Jan

[CFDKevin]

Originally Posted by hjasak

Hi,

My group at Uni Zagreb is running a project on added resistance in waves for large planning hulls. As a first step we did steady resistance (with sinkage and trim, obviosly).

We are using thd Naval Hydro pack with the wholg bag of tricks. The simulations run fine but we are stll learning about required meah resolution etc. Rhe forces on meahes of the order of 1.5 M cells are about 8% out, but I'm sure we will get better.

I think you have no chance with interFoam. It will ventilate, have a bad 6-dof solver (damping) and the interface jump conditions arent available.

Please send me an email if you'd like to hear more,

Hrv

Thanks for your reply!
It would be very interesting to know in some detail why Hydro Pack is better than interFoam/interDyMFoam. Also, if you could elaborate on the weakness of the 6-dof solver you refers to it will be much appriciated!

Originally Posted by JNSN

Hi Kevin,

simulations of planning hulls is definitely a challenging task for all CFD codes. Anyway, in my experience you can get very good results with interDyMFoam, and the 6DoF solver works absolutely fine for this.

I dont see the need to run interFoam in a first step. In order to ensure stability during start-up, you should ramp the forces. This option is available in the dev-Version:
https://github.com/OpenFOAM/OpenFOAM...7ec88e3cdb127a

For minimization of ventilation, a well designed mesh is necessary. Besides, there is an additional compression option together with an interfaceCompression-BC:
https://github.com/OpenFOAM/OpenFOAM...4ec11bb04bafb7

I have just done a small test with the new BC, and so far it looks quite promising.

Hope this helps,
Jan

Thanks a lot for your input on this topic Jan.
I have never seen the force damping ramp function or the interface compression-BC before, so I'm very glad you posted those. The force damping ramp function should be able to provide stability. Do you have experience with accelerationDamping to prevent large body motions from initial large accelerations?

[JNSN]

I think the most efficient way to reduce initial large accelerations is the force ramping. With a sufficient large ramp time you should have no stability problems (regarding 6DoF motion).
I have never used the acceleration damping, as most of the time I do transient simulations such as motions in waves, but may it can be usefull for such kind of quasi static simulations. Worth to try. But I can give no suggestion of appropriate values.
There some more options to increase stability of the 6DoF solver (and also help to converge faster to a steady state motion state):

1. Acceleration relaxation: the DTCHull tutorial uses a relaxation factor of 0.4; this should be already quite stable
2. Linear translation/rotation damper: these apply a force proportional to the motion velocity, for resistance simualtions including trim and sinkange this would be the heave and pitch velocity. The damping coefficients can be estimated straight forward from restoring forces.
3. motion solver: you have three options, sympletic (leap-frog), crank-nicolson and newmark. I have no experience with sympletic and crank-nicolson, but with newmark sovler you can introduce additional numerical damping by setting appropriate newmark parameters: see the link for a nice overview: http://opensees.berkeley.edu/wiki/in...Newmark_Method .

Best regards,
Jan

[vava10]

Dear Foamers,

I am working on a master thesis where I have to find the trim and sinkage of a kayak. This is the first time I am working with OpenFOAM, Linux, C++ codes and Ship simulations. So I am very new to the whole thing.

I did some research and found 2 methods.

1. Iterative method where I have to carry out the simulations at least 3 times for 1 velocity. I have to find the trim and sinkage for 2 velocities which would mean I have to carry out 6 simulations in total using interFoam. Unfortunately, I don't have enough time to do that.( I was trying to do that. I have generated the mesh and case file for this.)

2. Using interDyMFoam. A correct simulation would take 1 simulation for 1 velocity (at least that's what I think and I think if this is the case I might be able to find the results within the time I am allocated ). But I could not find any documents which describe how exactly the trim and sinkage is found using interDyMFoam. I did find a lot of threads in the forum but I still don't have any clear idea on how to find trim and sinnkage

Since everyone here seems to be well experienced in this field is it possible for you to PLEASE tell me how to determine trim and heave using interDyMFoam?

I would really appreciate it.

Thank you on advance and I am looking forward to your reply

Kind regards
vava10