Planing Hull Test Case
Hi, I am trying to look for a standard test case in planing hull (V-shaped).
Complete with the experimental data if possible (CFD result is fine also).
There are many other standard hull testcase, but I am looking into high speed regime and would like to simulate its dynamic trim and sinkage
So if anyone know whether such test case exist so I can do simulation to compare please let me know.
Or maybe other suggestion?
You should look for Savitsky. He developed some formulas to predict the speed of a planing craft using data from towing tank systemac series. you'll certantly find a huge amount of high quality experimental data.
Thanks for the reply, I am still trying to get my hands on those Savitsky paper, anyway I found this report by Gerard Fridsma, "A systematic Study of The Rough Water Performance of Planing Boats".
It does contain some free to heave and sink result on calm water and also the geometry of the hull (Constant deadrise and is not a typical planing hull that we see out there)
So in the meantime I will try to simulate this.
Hi, I have simulated some of the planing hull case now..
I am using Star-CCM+, but since my question is kinda general so I think I will just post them here.. :)
Let me explain my test case
Fridsma hull, with constant deadrise of 10 deg
Length (L)= 1.143 m
Beam (b)= 0.2286 m
Transom height = 0.143 m
Mass (m)= 3.6316 kg
I_pitch = 0.2965 Nm^2
CG location = 60%L from bow and 29.4%b above the keel
Test Speed = 1.5 m/s and 3 m/s
Free to move in vertical direction (heave) and pitch (trim angle)
I am trying to check my result with experimental data (in calm water) that the report provides. Some parameter that I would like to compare are Drag, CG position and pitch angle.
Up stream ~ 1L
Down stream ~ 2L
Side ~ 1L
Above hull ~ 1L
Below hull ~ 1L
Symmetry plane in the middle
Front, top, bottom and side is forced into Inlet (Velocity Inlet in Star-CCM+)
Back to Pressure outlet
Symmetry plane also for the midhull
Since I would like to get a feel of the simulation, I am trying to use a small mesh first, currently I am using about 500k cells with 8 processors running trying to avoid long simulation time. More resulution along the waterline, hull and wake is used
The simulation start by fixing the hull for the first 2s, then ramp it for 1s, and finally release it fully until a steady condition is achieved. Currently using Implicit scheme and segregated flow, realizable k-e turbulent model, with all y+ wall treatment.
In the simulation, y+ value looks fine, along the hull < 100
A few timestep that I used are dt = 0.01, 0.005, 0.001, 1e-8 with 15-25 iteration per time step
After monitoring the buoyancy, Drag, CG position and trim angle looks steady (small oscillation exist though) this initial result looks OK to me compared to the data despite small mesh is used. Nevertheless I am not sure about so many things, so please guide me :(
My problems are:
1. The residual convergence (all values I specified is absolute residual)
When the body is fixed, the first residual (momentum and continuity) on each time step is decreasing to 10^-4, but within the timestep it doesn't really decrease, say 1 order only. And after the body is free to move, it doesn't really decrease, it stays in 10^-4 but only decrease a bit no matter how many iteration I specified in each timestep. Some people says that it will be good to have 2-3 order drops in each time step, so does it means that my residual is not acceptable?
2. Timestep issue:
I notice that it is easier to make the residual drops using bigger timestep, 0.01 or even 0.1. But when I use small timestep such as 10^-8, the residual somehow keeps increasing after several timestep and I didn't continue it. Why is it using small timesteps leads to such behaviour in residual?
3. Using bigger timestep leads to unphysical phenomena which is the Hull is Flying above the water! Off course this is not acceptable. I notice that other people is experiencing with this issue, but using smaller timestep such as 0.001 is fine, at least it is not flying anymore. Checking the result when the hull is flying, the convective courant number around the hull is ~ 3 and when I use smaller timestep such as 0.001 I can get the courant < 1. My question is even using Implicit scheme in time, we still need to make sure the courant < 1 for planing hull problem?
Thanks before! ;)
Towing Tank results of hard-chine planing hulls:
calm water: http://eprints.soton.ac.uk/172717/1/...96preprint.pdf
head waves: http://eprints.soton.ac.uk/190035/1/...97preprint.pdf
hope this helps ;)
I have recently simulated a planing hull using a free surface multiphase model in CFX. I encountered air entrapment as well and was easily solved ensuring that the mesh at the free surface was very small 5mm in height for a 1.5m hull length.
My resistance results were very promising and flow fields matched also matched very well with my towing tank data and photos. The biggest variation occurred during the pre planing regime when the wave resistance is almost at its largest.
The free surface requires a very fine mesh above the expected (estimated) maximum height of your wave system produced by the vessel. I am very green to CFD so if anyone feels to add to this then great!!
air phase being formed on the bottom of the hull
hey buddy i am also facing same problem in planing craft that air phase being formed on the bottom of the hull.................how did u solve this problem.................reply as soon as possible...............
|All times are GMT -4. The time now is 07:19.|