CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Wave Simulation

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 1, 2011, 07:44
Default Wave Simulation
  #1
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
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
solimcfd is offline   Reply With Quote

Old   March 1, 2011, 09:46
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
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?
stumpy is offline   Reply With Quote

Old   March 1, 2011, 10:35
Default
  #3
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
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."
solimcfd is offline   Reply With Quote

Old   March 1, 2011, 15:21
Default
  #4
Senior Member
 
Join Date: Mar 2009
Location: Europe
Posts: 168
Rep Power: 8
joey2007 is on a distinguished road
Is the message from Pre or from the solver? If it is Pre try to activate beta features and to ignore.
__________________
-
-
-
-
-
------------------------------------------------------------------------
Please do not forget: I am not paid for answering your questions.


Thousands of issues can cause a division by zero. Please do not capture a thread, with the argument: "I have the same issue ...."
joey2007 is offline   Reply With Quote

Old   March 1, 2011, 16:01
Default
  #5
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
The message comes from Pre. I tried activating beta features but that didn't help. Thanks for the suggestion though.
solimcfd is offline   Reply With Quote

Old   March 1, 2011, 16:19
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
Try making the air phase dispersed. It shouldn't make much difference to the simulation.
stumpy is offline   Reply With Quote

Old   March 2, 2011, 04:59
Default
  #7
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
That did the trick, thanks for the help!
solimcfd is offline   Reply With Quote

Old   March 16, 2011, 04:48
Default
  #8
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
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:

FluidH is offline   Reply With Quote

Old   March 16, 2011, 06:00
Default
  #9
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
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!
solimcfd is offline   Reply With Quote

Old   March 16, 2011, 06:20
Default
  #10
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
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
FluidH is offline   Reply With Quote

Old   March 16, 2011, 06:31
Default
  #11
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
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.
solimcfd is offline   Reply With Quote

Old   March 16, 2011, 06:53
Default
  #12
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
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.
FluidH is offline   Reply With Quote

Old   March 16, 2011, 07:27
Default
  #13
New Member
 
Join Date: Jul 2010
Posts: 20
Rep Power: 7
solimcfd is on a distinguished road
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!
solimcfd is offline   Reply With Quote

Old   March 16, 2011, 08:19
Default
  #14
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
Sounds good. I will give you a notice if I get some results.
FluidH is offline   Reply With Quote

Old   March 30, 2011, 02:50
Default
  #15
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
ruirui389 is on a distinguished road
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.
ruirui389 is offline   Reply With Quote

Old   March 30, 2011, 03:03
Default
  #16
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
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.
FluidH is offline   Reply With Quote

Old   March 30, 2011, 03:11
Default
  #17
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
ruirui389 is on a distinguished road
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
ruirui389 is offline   Reply With Quote

Old   April 28, 2011, 22:38
Default CEL codes?
  #18
New Member
 
Join Date: Dec 2010
Posts: 19
Rep Power: 6
salvooch is on a distinguished road
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.
salvooch is offline   Reply With Quote

Old   April 29, 2011, 01:33
Default
  #19
New Member
 
Join Date: Mar 2011
Posts: 10
Rep Power: 6
FluidH is on a distinguished road
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.
FluidH is offline   Reply With Quote

Old   April 29, 2011, 12:06
Default
  #20
New Member
 
Join Date: Dec 2010
Posts: 19
Rep Power: 6
salvooch is on a distinguished road
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!

Last edited by salvooch; April 29, 2011 at 18:19.
salvooch is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
what is the condition to use the wave equation? mmff Main CFD Forum 0 January 26, 2010 05:25
Continuous vs interrupted simulation sega OpenFOAM Running, Solving & CFD 4 November 3, 2008 15:29
Breaking Wave Simulation Mehdi BEN HAJ Main CFD Forum 2 February 12, 2002 12:07
Breaking Wave Simulation Mehdi BEN HAJ CFX 0 February 9, 2002 13:34
Breaking Wave Simulation Mehdi BEN HAJ CD-adapco 0 February 9, 2002 13:32


All times are GMT -4. The time now is 01:09.