Hi everybody,

Actually, I am working in a research project in the Instituto Superior Técnico (Portugal), and now I am trying to simulate the flow around a ship hull form to calculate: the skin friction resistance, viscous pressure resistance and the wave making resistance using CFX program. In fact, I need help in the following points:

1-What is the exact condition at the outlet boundary (I have tried to apply the atmospheric pressure at the outlet boundary condition, but there is always a warning message with the outlet boundary condition and it cases some errors in some cases, so how can I prevent this).

2-When I am trying to obtain from the post processor of CFX the calculated force on the hull form in X direction, I always find the forces excreted by air and water are of the same values, also the same case for the shear stresses, and there must be a difference between the values, so what are the mistakes here and why the results are the same for the two fluids.

3-How can I get the value of wave making resistance, viscous pressure resistance from the post processor of CFX.

Please, I need the help in this parts too much, and many thanks for everyone in this forum.

Based on my experience with the CFX here are my answers:

1) You should not define the atmosphereic pressure at the outlet bounday but infact you should define the hydrostatic pressure based on the intial water height at the outlet

2) I think your Bounday conditions are wrong thats why youre geting the same forces. try using the above mentioned outlet BC and see.

3) When you run the solver after the the end of your simulation it prints out the Pressure(wave) resistance and Viscous resistance individually in all the directions.

Hope this message is of any help for you Good Luck

Many thanks for you Sir. Now I am trying to apply these useful notices.

Yours,

Yasser

You will find page 191 of the CFX Modelling manual very helpful for how to specify your outlet boundary.

Also be aware that for correct wave making resistance calculations you need a very fine mesh (order of 10 mm vertical) on the surface and *very* long simulation runs for wave shapes to propagate through the domain.

/C

Wave making resistance and pressure resistance are not equal!

Hi

Many thanks for everyone who gave me a help, I really appreciate that too much. In fact, I wish to ask some questions:

1- I have put nearly 1.5Ls (Ls = ship length) forward of the bow, 2Ls aft of the stern and Ls is the width of my domain (the domain in cylindrical and I have taken only one half of the domain due to symmetry), is this enough for simulating the flow with free surface around a ship hull form? 2- I have used the same equations in CFX tutorial 7 to define the hydrostatic pressure at the inlet and out let, is this correct? 3- I don not have the height of the fluid at the outlet and I have taken it to be the same as the input height for defining the equation of hydrostatic pressure at the outlet boundary, is this right or how can I overcome this problem? 4- Which is better dealing with this problem as a transient problem or as a steady problem using the Mesh Adaption option, because I have used the last option but I always find wrong values for the forces (pressure and viscous forces) and in the shape of the interface surface between the two fluids (wave pattern). 5- The pressure force is the sum of wave making resistance and the viscous pressure resistance how can I obtain the value of each one from CFX.

Please, I need help to this point as soon as possible.

Many thanks for everyone.

Yours,

Yasser

RE : Wave Making resistance: ( Please Correct me if I am wrong)

Yes viscous pressure resistance and wave making resistance are different but in CFX when you calculate the pressure resistance it combines both the wave making and viscous pressure resistances. I dont know any way to calculate them individually. About your outlet conditions you basically defnie the outlet water height as same as inlet one's and allow the solver to compute the water level.

I dont think CFX mesh adaption is robust enough to calculate the wave height. so I would rather try to make mesh very finer in those regions were I expect to find the interface region.

The steady state solution is hard enough to get right, you know! And unless you want to include environment waves in your simulation you dont need transient.

I belive the area integrating functions such as force_()@... and torque_()@... etc include both the pressure and shear forces. So if your ship is moving along the x axis the resistance is just force_x()@Hull (if Hull is a region with all the surface elements from the hull). Eh, make that 2xforce_x()@Hull if your half-symmteric

2L after the stern is not enough usually. You will see faster convergence if you make it longer, say 4L minimum. Even though you have more nodes the solution will converge quicker because there are less reflected disturbances from the outlet.

/C

[jhao0]

Hello, I am also interested in your research. Actually, I am going to simulate the wave-making resistance in different Fr for a ship model. But, I don't know how to determine the expression of wave-mating resistance in CFX. Could u please share the expression with me? Thank you very much.