Problem in determining lift coefficient using Fine Marine

Hi Marcar,

When creating a mesh with the 2D option, there is only one cell in the thickness direction, but this is due to the geometry thickness and is artificial.

As expected, the solver will see the grid as purely 2D, meaning with no thickness. As such the forces you see are in fact lineic, expressed in N per unit of span. This is why when you calculate the lift you replace the foil surface S by the chord (a length) and you still obtain an non-dimensional coefficient.
Best regards,

Lucas

Thanks for the reply,
I have a doubt because in the case that I am replicating, the Duncan's experiment described in the paper (www.researchgate.net/.../356567405_Free-Surface_Effects_on_Two-Dimensional_Hydrofoils_by_RANS-VOF_Simulations) and carried out with Fine marine, I obtain a lift and therefore a Cl equal to about 1.3 which is very high also because I am at Re even at 1.59*10e5.
I made a mesh with about 40,000 cells and use the AGR with the Free surface tensor to refine the free surface.
The time configuration is steady, the solver is k-omega (SST - Menter), the boundary conditions are farfield for the inlet with the speed obtained from Reynolds, then on the top and outlet prescribed pressure with updated hydrostatic pressure and on the bottom wall with slip condition . I impose initial conditions with the speed I get from the Reynolds.
What do you think I could have done wrong in this setup?
thank you
best regards

Thanks for the reply,
I have a doubt because in the case that I am replicating, the Duncan's experiment described in the paper (www.researchgate.net/.../356567405_Free-Surface_Effects_on_Two-Dimensional_Hydrofoils_by_RANS-VOF_Simulations) and carried out with Fine marine, I obtain a lift and therefore a Cl equal to about 1.3 which is very high also because I am at Re even at 1.59*10e5.
I made a mesh with about 40,000 cells and use the AGR with the Free surface tensor to refine the free surface.
The time configuration is steady, the solver is k-omega (SST - Menter), the boundary conditions are farfield for the inlet with the speed obtained from Reynolds, then on the top and outlet prescribed pressure with updated hydrostatic pressure and on the bottom wall with slip condition . I impose initial conditions with the speed I get from the Reynolds.
What do you think I could have done wrong in this setup?
thank you
best regards

Hi,

First, as your predicted lift coefficient is twice higher than the one mentioned in the article, make sure that you are using the actual chord to calculate the C_L. 

Then, the setup should be check to make sure the conditions are identical:

• Angle of attack of 5°
• Correct free surface height (so that immersion expressed as fraction of the chord is identical)
• Correct depth
• Reynolds number is correct

For AGR, it would be interesting to check the free-surface discretization to see if the AGR parameters you have chosen are correct, in the article the recommendation for the Free surface tensor target cell size is c/100. 

Finally, in the monitor make sure that the forces are well converged and that the computation has not been stopped too early. 

Those checks should help you to find the issue, such a difference for a converged value is usually related to a difference in the set-up.

Best regards,

Lucas

Hello,
thanks for the reply and for the help. I checked the simulation in all the aspects you mentioned, but unfortunately I can't get the desired result, the lift is always around 80 N, so the lift coefficient is equal to 1,20 (double what I should get).
I noticed that if I decrease the speed (even to 0.001 m/s) I still get a lift equal to 34 N, which is strange. Would it be possible to share the simulation for better understanding? Or is there some tutorial or documentation I can follow to figure out where I'm wrong?

Thanks a lot and best regards,

Marco

Hi,

We do not have a Demo case that reproduces this particular set-up. Regarding the troubleshooting, below is a path you can follow.

If with a neglectable speed you still get lift, it means that the simulation is setup incorrectly and that there is a flow close to the hydrofoil. 

- Check in initial solution that you also updated the speed to 0.00 m/s

- Check in body motion that every degree of freedom is set to "fixed", if you impose a motion in this menu the foil will move inside the fluid at rest which will generate lift.

- If  the points are correct, then you can move on to CFView on the on your computation with the low speed, where you can display the X component of the velocity vector. Check it indeed matches the speed you want in the far field. 

Kind regards,

Lucas