[doyal kumar]

Hii
I would like to predict total resistance coefficient and wave profile along the Wigley hull in STAR-CCM+. I am having some problems with my simulation.
I have created a force coefficient report but what would be the reference area in properties bar? Or is there any way to calculate the wetted surface area of the hull?
I am using a flat vof wave and DFBI model which is free to sink and trim. I want to create a wave profile along the hull, but don't know what to do.
Any advice would be a great help. Thank you.

[ping]

create a sum report using the area field function in the direction required to get the projection hull area

wave profile can be made by creating an isosurface of the volume fraction of water at 0.5 but use the hull surface as the input part rather than the full region

[doyal kumar]

Ping, Thank you very much.
Now I am clear about the reference area. But one more question on wave profile, if I select full region as input part, I get the a wave pattern and by activating isoline labels also get the value of position[z] on the isosurface but there are so many value. Now my question is, how can I get the value of position[z] just on the surface of the hull so that I can plot a graph wave height vs length of the hull. For convenience, I am attaching an image of wave scene. Again, thanks for helping me.

[ping]

you have not followed my answer since you have used the full domain as the input part for the isosurface

you need to replace that with just the hull boundary and this creates the intersection of the wave and hull which is a line

and rid the iso labels and just use a normal smoothed contour

and if you have modeled the full hull rather than half then to rid one half you can clip the scene displayer in the y direction

[doyal kumar]

Sorry I was mistaken. Now I have created an iso surface with the input region just hull. Here are my steps
open a scalar scene with above mentioned iso surface as part and assigned the position[z] as field function.
Got the intersection line as you said but by activating iso labels there were no value on that intersection line. though there is a color bar that indicates the value of position[z] but it is quite difficult to point out the exact location on the line.
could you please explain further.
Thanks.

[ping]

looks like you have the wave profile now so to have just a line with no scalar colour etc place the isosurface in a geometry displayer and then you can control its features and remove the scalar displayer

if you want the profile displayed on a plot then create a new plot and ass the isosurface part to the plot and set the required axes eg x as position x and y as position z

[doyal kumar]

Thanks a lot, ping. My problems have been solved. Without your direction, it wouldn't be possible.
One more question, I know the procedure how to normalize the scalar function. If I want to normalize vector like direction [1,0,0], what will be the procedure?

[ping]

for your vector question it is time to read some of the extensive help on field functions

[zyfsoton]

Originally Posted by doyal kumar

Thanks a lot, ping. My problems have been solved. Without your direction, it wouldn't be possible.
One more question, I know the procedure how to normalize the scalar function. If I want to normalize vector like direction [1,0,0], what will be the procedure?

Hi Doyal, I am facing the same problem as yours. Currently, I am hoping to plot the wave profile along the hull in Paraview but I cannot manage to do that. Could you please share some steps for doing that? Many thanks, Tony

[ping]

why would you use paraview when it is so easy in star?

[zyfsoton]

Originally Posted by ping

why would you use paraview when it is so easy in star?

Hi ping, since I am using openfoam6 to run the case and postprocessing in paraview instead of starccm+, do you have any idea of how to do this in OF? Appreciated it if you can share something. Thanks, T

[doyal kumar]

Hii,
I didn't use the Openfoam but used Starccm+. And I never used the OpenFoam, so I am afraid whether my done steps would be any help or not.

[ping]

Originally Posted by zyfsoton

Hi ping, since I am using openfoam6 to run the case and postprocessing in paraview instead of starccm+, do you have any idea of how to do this in OF? Appreciated it if you can share something. Thanks, T

i know nothing about paraview, but i would hope you can do it in there too.
the result you want is a line at the intersection of two surfaces - one is the hull which you already have and the other is an iso-surface of the air-water interface and this is normally an iso-surface of the water phase at 0.5 concentration.
as the how you intersect these surfaces i suggest you ask a paraview forum.