CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Wave Simulation (http://www.cfd-online.com/Forums/cfx/85552-wave-simulation.html)

solimcfd March 1, 2011 07:44

Wave Simulation
 
Hi, I am using CFX to model ocean waves using linear wave theory. I am using a multiphase simulation with air and water as the fluids. My results seem reasonably good but I would like to inject particles into the flow in order to see how they move in the field and to compare these particle tracks with theory. My problem is that I cannot add a particle transport solid if I already have two eulerian fluids, CFX doesnt allow it. Does any one have an idea of what I could do? Thanks

stumpy March 1, 2011 09:46

What version are you using? I've seen particle track + free surface simulations, so it can be done. Perhaps only for homogeneous multiphase? Perhaps only in the most recent version?

solimcfd March 1, 2011 10:35

I'm using CFX 12.1 with the homogeneous multiphase phase model, but when I try to add the particles I would like to track the following message appears:
"particle tracking simulations with more than one continuous Eulerian phase are not supported."

joey2007 March 1, 2011 15:21

Is the message from Pre or from the solver? If it is Pre try to activate beta features and to ignore.

solimcfd March 1, 2011 16:01

The message comes from Pre. I tried activating beta features but that didn't help. Thanks for the suggestion though.

stumpy March 1, 2011 16:19

Try making the air phase dispersed. It shouldn't make much difference to the simulation.

solimcfd March 2, 2011 04:59

That did the trick, thanks for the help!

FluidH March 16, 2011 04:48

Hi!

Sorry for asking You some questions in your post.
I am trying to make the same analysis as You, modelling linear waves in a 2d numerical wavetank.

I do not get any good results, so I am very interested in your setup and boundary conditions in CFX Pre.

My main problem is the large dissipation along the tank. Do you achieve little damping ?


Here are a graph of my results:

http://folk.ntnu.no/jarlehav/pics/WaveElevation.png

solimcfd March 16, 2011 06:00

Hi! I have tried two different methods to produce waves. First I used an inlet with specified velocities from linear wave theory and the other method was to use a deformable mesh that acts as a wave maker. Both methods create waves but I have the same problem as you with damping. I am still working on this problem but from what I see refining the mesh in the wave propogation direction and decreasing the timestep seems to improve results. Maybe we can try and work together and solve this issue!

FluidH March 16, 2011 06:20

Hi!

Thanks for fast reply;-)

I also just saw your other post regarding waves in cfx, should posted it there maybe.

I have also used a linear velocity field at the inlet with just an entrainment opening at the outlet with static pressure at mean water level.
In this case I also tryed to set up initial conditions with a wave profile in the domain. This helps starting the solver if convergence problem.

In addition I also have simulated a piston and flap wavemaker with moving mesh.
Here the piston wavemaker seems to gives reasonable results. (Better compared with the velocity profile). But also here the problem is the dissipation along the tank.

I also have tryed to run with a physical beach with slope 1:10 to reduce reflection. Latest I have tryed with a artificial damping sone with a momentum loss modell.

But the main problem is still the dissipation along the tank.

Running with dt=0.01s with courant number just below 1.
Using High order or specified blend =1 for the advection scheme and 2nd order backward Euler as transient scheme.
Convergence criteria RMS =1e-5. Min 3 coeff loops and max 6 coeff loops.



Regards

solimcfd March 16, 2011 06:31

Yeah, I am also using a physical beach, this does help with reflection but does not change the damping. What kind of grid are you using? Have you refined it in the region where the free surface is? What I noticed is that the damping gets worse when the cells are stretched quite a lot. There is a paper that has investigated all of these problems: http://www.ipen.org.br/Artigos-congr...NA2010-141.pdf. I am trying to reproduce their results, but for some reason I get excessive damping.

FluidH March 16, 2011 06:53

I also have the same paper on my desk, trying to get similar results.
Instead of a hinged flap I have used a piston for simplicity.
Regarding the mesh I use a refined region close to the free surface with similar mesh refinement as recommended in that paper. Some improvement as been achieved when the mesh was refined in the longitudinal direction.

Do you use parallell computing? I have noticed some problems with parallell run.

solimcfd March 16, 2011 07:27

No, I have only tried serial up till now. Ok, so lets stay in touch, if I find out anything else I will let you know. Thanks!

FluidH March 16, 2011 08:19

Sounds good. I will give you a notice if I get some results.

ruirui389 March 30, 2011 02:50

hi i'm not a CFX but a FLUENT user. i saw the time of your image is t=20s. does it still decrease so much after 100s? and i saw your wave length is quite small (around 2m), what about long waves? besides, perhaps u can modify the viscosity of water.

FluidH March 30, 2011 03:03

Hi!

Yes I know I am running small wave lengths. The reason is that I want to compare my results with experiments in a wave tank with a depth of 1m.
So to have linear deep water waves I have used 1.5m and 2m wave lengths.
With longer wave lengths I have achieved some better results.

After about 25s I get reflections from the outlet wall (beach with 1:3 slope).
So thats why I haven't run any longer.

Regarding the viscosity I would like to keep it similar to water viscosity.
To obtain wave forces on submerged structures the viscosity needs to be similar as experimental setup.

ruirui389 March 30, 2011 03:11

yes the reflections is really a problem. in my opinion the shorter wave energy decreases faster than long wave especially at the beginning. perhaps u can enlarge the length of your wave tank to earn more time

salvooch April 28, 2011 22:38

CEL codes?
 
Hi, I'm trying to make a flap-type wave maker, but am having a hard time generating the expressions for this boundary motion. I am able to do the piston-type, just can't get the flap-type to work. Anyone able to pass the CELs to me for the flap-type boundary?

Thanks.

FluidH April 29, 2011 01:33

Hi, Flap type is almost similar as piston type. Only difference is the amplitude which will variate along the z-axis (vertical).

For a bottom hinged flap:

flap_motion = A*((z+h)/(h_domain))*sin(omega*1.[rad]*t)

Here A is the amplitude at top of domain, z vertical coordinate, free surface at z=0,h= water depth and h_domain the total height of domain ( water and air).

The amplitude A is sometimes described by S = piston stroke at free surface.
(S=2*A_surface).

For a hinged flap, just use a if function with no motion below the hinged point.

salvooch April 29, 2011 12:06

Thanks! I got the wall to move, but the wall height below the hinge isn't remaining stationary. It's like it is pivoting about a hinge, but pivoting on both sides... and the wall swings upside down (meaning it hinges at the top). Any additional help would be greatly appreciated.

Again, thanks for all help to get here! Still further along than I was yesterday!


All times are GMT -4. The time now is 13:36.