Drag Predication Problem for free-surface flow using STAR-CCM+
 

Dear all,
I am currently doing test-validation cases for free-surface flow [VOF method] over a Wigley Hull geometry using STAR-CCM+ v5.06.

For a contant Froude Nb. = 0.267 case, the solution is converged, and also the maximum and area-averaged CFL numbers on free-surface look great too (below 0.1 and 4 respectively). The total drag force is also coming in a good range of agreement. The water-line at hull surface matches with experimental data.

The only issue is that even after t = 35s of physical simulation time (and time-step of 0.01s), the drag forces keep oscillating with 1 N range for presumed steady-solution. Even though drag force range is small value, when calculating drag coefficient and try to compare with experimental data; the difference is huge about 10-15% error.

P.S. I used reliazable K-Epsilon two-layer turbulence model [with required sufficient viscous boundary layer mesh resolution (y+ = 1) on the wigley hull surfaces].

Please advise on how to increase the accuracy at calculating drag force.

Thanks.

it is very common for vof marine calculations to oscillate even after long run times - depends on many factors like DOFs freed, MoI, wave interactions and reflections etc etc. Ensure you have suffucient inner iterations, and dt is small enough. Then if the variations seem logical, simple average the drag results - eg use field mean monitor with a sliding window (or export drag monitor to Excel etc and average there).

I agree with your concern, but my simulations are with 0-DOF and calm incoming water (no waves). The time-step is 0.01s with 25 inner iterations.

Drag Measurement
 

Since this validation case seems to be mostly working for you, I thought I'd add a question. For measuring drag, are you doing anything more than setting up a force (and/or coefficient ) monitor for the vehicle body in the direction of current? (Fx typically)

I'm primarily an aero guy, but just started running some VOF simulations for a (just barely) submerged body at increasing distance from the free surface. The goal was to look at wave drag as a function of depth, and we were expecting to see some increase as the vehicle approached the surface and expecting an exponential relationship. The Froude number is 0.4 so there should be a lot of wave drag. We get pretty reasonably looking surface perturbations, which do increase significantly as the vehicle approaches the surface, but the drag is absolutely steady, and varies by only small fractions of a percent between depths, with no trend to depth at all.
thanks
M<

probably it is not the cause, but...

to perform the drag evaluation are you considering only the water phase's drag or also the air one?

@ matt:

you shoud not expect grat variations because the wave train you obtain is generated by the pressure field wich encounter the free surface.

I'm just creating a force report (Pressure + Shear) on the submersible body. Is there a better way to capture the physics?

Who says, the oscillation is not physical? There are not very much real steady flows. Usually you can see osciallations due to vortex shedding in a lot of applications, and very often the oscillations are too big to neglect. O.k., 10 to 15% is a lot, but I wouldn't be too worried about the oscillations itself.

When you put a body in a wind tunnel (or a hull in a water channel) to measure the drag, your measurement system will usually average the values over time and it seems, there would be a steady flow.
Just consider a karman vortex street behind a cylinder, like a chimney, an antenna on a car roof or a house.

Got something very similar
 

i am running a tow tank equivalent simulation.
hull fixed.
speed - 2.1m/s length of hull about 6m.

size of water domain - X=16m Y=9m

for the shear force i get the exact tow tank result. it looks very stable.

for the pressure force i get an oscillating force between 10 and 3, which gives the mean value of 6.5N which is not bad compared to the tow tank result.

i have a "pressure outlet" condition on the outlet wall.

is the oscillation a result of reflected long wave?

how can i solve it? (will the wave decay if i make a gradual enlargement in the width of the domain far behind the hull?)

thanks.

Hi Surfboy,
Q: Is the oscillation a result of reflected long wave? how can i solve it? (will the wave decay if i make a gradual enlargement in the width of the domain far behind the hull?)
A: Yes. Bigger domain helps this problem. Also, Once you get started converged solution, you may increase under-relaxation little bit and run faster for few more iterations to get low residual results. From this exercise, I found drag forces to be stable.

the pressure drag fluctuation seems way too high (assuming you have run for quite a long time), especially since the hull is fixed. a larger domain might help as will dampening the waves at the boundaries - use the boundary wave dampening feature and maybe coarsen the mesh up (slowly since rapid size changes can also cause reflection) towards the boundaries (by not the inlet).

train moving in tunnel help
 

hello
i am working on train moving in tunnel. i am getting floating error:invalid number. can any one help me. my email is sheikhnasir39@gmail.com
plz help me
thanks

:confused:

What does your problem has to do with freesurface flow? :mad:
Why do you post the same post about thirty times anywhere at the forum? :mad:
Do you want me to inform the adminstrator about your spaming?! :mad:

As you can see, nobody can help you. And do you know why?!
Because your post is so meaningless that nobody could ever help you. So please, be more specific or leave it and especially dont spam the forum, maybe then anybody will help you.