# Free Surface Ship Flow

 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 24, 2013, 07:22 FixedAxis constraint #221 Member   carlos Join Date: Apr 2011 Posts: 37 Rep Power: 14 Hi all, Is there any way to specify the axis position in the six dof constraint, as it is done with fixed line, in which there is a reference point?? So far, specifying the vector (0 1 0) allows rotation around Y axis, but rotation occurs arround coordinates origen. Of course I can displace the body to put the turning point in coincidence with the CO, but it is complicated to re-mesh all geometry just to move the rotation point. Thanks in advance, Carlos.

 May 22, 2013, 11:04 #222 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 Carlos, You can specify your reference points by using "refPoint" under "fixedLineCoeffs". Please see the example code below: fixedLine { ... ... ... fixedLineCoeffs { refPoint (1 0 0) direction (0 1 0) } } I haven't tried this for rotation but I think the same thing works for "fixedAxisCoeffs" too.

 May 22, 2013, 12:32 #223 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 15 Hi all, Just because I'm curious....does anyone over here, other than myself, has a working OF development in which a sailing ship can be simulated? @Kilroy: I'm sorry, I'm not really familiar with the RefPoints. Regards, Ralph __________________ CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html

 May 22, 2013, 12:46 #224 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 Ralph, That's what I am working on right now. I am trying to simulate a ship with 6DOF under the effect of waves by using waveDyMFoam. waveDyMFoam is a derivative of interDyMFoam which has been developed by Niels Gjøl Jacobsen. I am having a lot of trouble with the mesh right now but hopefully I will make it work soon. Thanks,

 May 22, 2013, 14:33 #225 Member   carlos Join Date: Apr 2011 Posts: 37 Rep Power: 14 Thank you for the answer Kilroy, but I have solved the issue some time ago. Ralph, I have been looking to your F18, and I am curious on the solver you have used to manage the vertical movement, I have been working with a speed boat and managed up to 37 kn (for 12 m lwl) amd 2 dof, but needed a very corse mesh. Since I tested the real boat, I can tell that the trim results and wave formation is good, but the results of forces are bad. (waveDyFoam) Also tried to use the trim with the LTSI solver but the problem is the vertical movement limitation. In the video of the F18 it appears that you start with a speed the is being increased later. I had that in mind to reduce the shock of a sudden start at high speed but did not know how to do it. Thanks, Carlos.

 May 22, 2013, 17:04 #226 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 15 Carlos, Nice to see your involvement. I'm using a modified version of shipFoam. The mesh in the video is a bit coarse since I haven't unlimited computation power. At that time only trim was included but right now I'm also performing dynamic trim simulations. These are highly unstable so require a special treatment. The F18 simulation is started at a fixed position for some time, then trim is activated. I was thinking to include a velocity ramp but this is quite some work, with my current setup I think I don't need this setup anymore. However, it would certainly a better starting point! Adios! __________________ CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html

 May 22, 2013, 17:10 #227 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,898 Rep Power: 36 Hi Carlos, Since you are using waves2Foam, I suppose you would be able to accelerate the steady flow in a gradual manner by setting Tsoft to an appropriate number in waveProperties.input. Kind regards Niels

 May 24, 2013, 10:30 #228 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 I am trying to model a ship traveling in the ocean through the waves with constant speed. At first, everything seems to be alright in the simulation. But after some point, the oscillations of the ship in the direction of gravity seems like getting higher and higher (the vehicle sinks more and jumps more on the water as the simulation progress further). You can find a video of my simulation attached. http://www.filedropper.com/vehiclewaves I checked everything but nothing seems wrong. Still the ship is unstable. I can put some restraints and constraints but how realistic would those be? Do you have any suggestions to where to look at in my model? Or how to fix that problem? Kilroy

 May 30, 2013, 08:18 #229 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 15 Kilroy, I think the mesh is too coarse resulting in no viscous damping and possibly a time step for the calculations which is too large. So you have 2 options: -decrease cell size near your ship -decrease time step size and apply artificial damping (not sure if that's possible?) Regards, Ralph __________________ CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html

 June 23, 2013, 08:11 #230 New Member   Tim Join Date: Dec 2012 Posts: 7 Rep Power: 12 Hey there, I try to simulate a riverboat with 2 DOFs (pitch+translation z) in flat water conditions. So far I got an errror about 10kN from simulation data to experimental data. I checked the mesh and the boundary conditions but everything seems fine. Also I change the solver settings and the temporal discretisation, without success. Maybe this depends on the coordinate system? Does anybody know about the reference coordinate system for resistance measurement? I am happy about every hint .... Regards Tim

 June 23, 2013, 09:26 #231 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 Hi Tim, If you can upload your case, I can try to help. Sincerely, Kilroy

 June 23, 2013, 15:46 #232 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 15 Hi Tim, First of all it would be interesting to see the relation of error in comparison with the total resistance. Furthermore, since you have model experiments and an estimated wetted area, you would be able to decompose the experimental data into pressure and viscous resistance. This should give you more details on where to look for errors. Which kind of solver are you using? What is your y-plus value and did you performed classical benchmarks such as a flat plate (viscous resistance) and wigley hull? I've got more questions ready for you . Cheers, Ralph __________________ CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html

 June 24, 2013, 04:00 #233 New Member   Tim Join Date: Dec 2012 Posts: 7 Rep Power: 12 Thanks for your fast reply.... First of all, I use Star-CCM+ to simulate the riverboat. Before I started to simulate the boat with free surface I do some Double-Body test to estimate the resistance (shear+viscous pressure) and check the turbulence Models and y+ values. The produced error was around 3-5%. The y+ value was around 50-150 and the SST-Model did the best job (as expected). So far I use implicit and explicit solver to simulate the boat in flat water conditions (VoF model). The implicit solver produces the smaller error. Also I do some further refinemnets and check the Moments of Inertia with NAPA. The error is around: - 2% - 3.5m/s -12% - 4 m/s -16% - 4.5m/s -17% - 5m/s Last edited by TSC; June 24, 2013 at 05:14.

 June 24, 2013, 10:47 #234 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 Tim, This is the OpenFoam forum. If you go to Star-CCM+ page and post your problem there, you can get help form Star-CCM+ experts. Sincerely, Kilroy

 June 24, 2013, 12:01 #235 Senior Member   Ralph Moolenaar Join Date: Aug 2010 Location: 's-Hertogenbosch, the Netherlands Posts: 120 Rep Power: 15 Tim, This sounds like a refinement issue (to capture wave details, check if waves are described by at least 10-15 cells) or a difference in trim/sinkage which can cause significant differences. As Kilroy stated you should be able to get better help at the StarCCM-forum. Good luck! Ralph __________________ CFD for marine applications? Go to http://www.marinecfd.com/ and join the OF Ship Hydromechanics Group: http://www.cfd-online.com/Forums/gro...mechanics.html

 June 25, 2013, 03:21 #236 New Member   Tim Join Date: Dec 2012 Posts: 7 Rep Power: 12 Dear Ralph and Kilroy, I konow this is the OpenFOAM Forum, but I think this problem isn't because of the software (and the support at the Star forum isn't that good ). @Ralph: I also think this is because of the trim. The sinkage is the same than in model tests. But I don't have any detail information about MoI or CoG. I try to calculate this with NAPA, but who knews the configured CoG by the model basin. This may cause the error....

July 15, 2013, 04:38
#237
Member

Join Date: Apr 2013
Posts: 32
Rep Power: 12
Quote:
 Originally Posted by TSC ...So far I use implicit and explicit solver to simulate the boat in flat water conditions (VoF model). The implicit solver produces the smaller error..
Are you referring to if the transport eq. for the volume fraction is solved implicitly/explicitly?

If so, (this is a question for everyone), does implicit solving of the alpha1 in OF yield lower error as well? ShipFOAM solves implicitly for alpha1, while interFOAM is explicit by default.

Best regards, simt

 July 24, 2013, 02:35 #238 Member   Join Date: Apr 2013 Posts: 32 Rep Power: 12 I've experienced a (oscillating) pressure resistance when using interFoam for free surface hydrodynamics. Pressure oscillates about +- 20 % with periods of ~4 seconds, anyone knows the reason for this?

 July 24, 2013, 09:54 #239 Senior Member     Join Date: Mar 2013 Location: USA Posts: 120 Rep Power: 12 Smit, Oscillating pressure values for the first few seconds is normal. Try to run your simulation for 60~80 seconds. Then take the average after the system gets into steady-state. If the pressure still oscillates even after the 80th second, then you may consider decreasing your time-step. If that doesn't help too then you can try refining your mesh. Let me know how it goes Best Kilroy

 July 24, 2013, 10:39 #240 Member   Join Date: Apr 2013 Posts: 32 Rep Power: 12 kilroy, thank you for your reply. I'm simulating a model ship of 6.5 m length at a speed of 2 m/s. Is it normal to find oscillations of fairly constant amplitude and period time from simulation time ~10 s to 30 seconds? It is barehull (half hull) and I'm using 2.5M cells currently. I will continue to simulate to see if the oscillations vanishes. Best regards, simt