[PeiSan]

Hi,
Question 1
I run the resistance simulation for my hull to compare with the experiment data. However, the data produced by fine marine is still not match with the experimental data. I already do my setting for my hull (1.372m) as listed below:

In Hexpress;

Global refinement = 8
Refinement for hull = 5 (tick target size cell)
Refinement for transom = 6 (tick target size cell)
Internal surface = 8 (target size cell is 0.2(for X&Y) and with aspect ratio of 200)
y plus = 1
stretching ratio = 1.2
No. of layer = 10

In Flow Solver;

Reference length = 1.372m
Reference velocity = 0.32067m/s
This parameters set to make a constant Reynold number (Laminar)

Final velocity (body motion) = 1.029754m/s (1/2 sinusoidal ramp)

The percentage of error is still big enough between the CFD and experimental data.

Question 2
After that, as i increase froude number to run with my model, the percentage error of the data between the CFD and experimental become more bigger in value.

Is it my setting for mesh or flow solver part wrong that lead to wrong data produced? ( I have already increase the mesh number to 3 million and increase the refinement number). Any suggestion or idea to solve the problem?

Thanks.

[Rombzh]

Hi,

1) What kind of boundary conditions did you use for the hull surfaces ?
Also why did you use v=0.32067m/s as your reference velocity (to compute Reynolds number and then I assume the spacing to get a y+ of 1), while the hull is going at 1.029754m/s ?
Check the y+ value on the hull in Cfview.

Is your free surface resolution (in X and Y plane) good enough to capture the wake ? Check the free surface elevation in Cfview.


2) If you kept the very same mesh but for different velocities, it is likely that your original viscous layer spacing is off (and it might even be wrong in the first place).

[PeiSan]

Hi Rombzh,

1) For hull surfaces (hull and transom), i set them to wall-function while deck as slip.

In flow model, i set v=0.32067m/s as my reference velocity because i want to make a constant reynold number in order to produce laminar flow. While, the hull is set to 1.029754m/s because i want my hull to going at this constant speed. Is that wrong where the reference velocity and the final velocity (hull speed) must be the same? If i put 1.029754m/s for reference velocity and the final velocity, the data is still have error but not have big value of error as i using difference value for those two velocity.

While for y+ value, In Hexpress Viscous layers, i put the value as listed below to compute the first layer thickness;

y+ = 1
reference length = 1.372
reference velocity = 0.32067m/s
Kinematic viscosity = 1.1e-006

2) The original viscous layer spacing is it corrected by increasing the number of layers

Thanks

[Rombzh]

Hi,

If you're targeting a y+ value of 1 you should not use Wall Functions but "No Slip Wall" for your hull boundary conditions. For the deck, free slip is fine.

In Flow Model, the Reference Velocity is only used to compute the time step, that's basically it. But if you used v=0.32067m/s as a reference to compute your Reynolds number and then the spacing that will get y+=1, this is wrong.
You need to specify the final velocity the hull will travel at, so here v=1.029754m/s.

[PeiSan]

Thanks Rombzh, i will try your suggestion.