[arun7328]

Dear All,

I am going to work on wave interaction on ships and the dynamic forces for various cases. Just to get the modelling and meshing right for VOF wave and to what comes out of the software for a user defined wave, I am simulating first order waves in a rectangular domain.

The domain is 75m(x), 10m(y which is the direction of wave height), 1m(z direction). The free surface is initialized so that the domain is equally divided. The coordinate of y axis of free surface is 0.

I have defined a wave of length 5 mts, current/wind velocity 1.5 m/s, amp 0.1 mts. The mesh sizes on the free surface is refined using a block of height 0.3 m. The x and z refinement are wavelength/80 and y axis is amp/20. Time step is wave period (2.4*80). I have run the simulation using 50 and 70 inner iterations but the nature of the pressure plot seems to be that of a damped oscillation. Though the waves are not becoming completely flat , which was an issue i had before, it gets damped a little. The point on water level of the wave is 0,0,0. The distance from the wave to outlet is 50mts.

I have also changed the VOF relaxation from 0.9 to 0.5 but there is no change. Can anyone please guide me regarding what is going wrong or what other parameter i could change. I am running unsteady, inviscid model and 1st order solver.

Thanks
Regards
Arun

[saeed.barzegar.v]

Dear Arun

I had a same problem. I suppose, you are working on old version of fluent? if it is true, you can follow another simple way (by new version of fluent (in ANSYS 13 or 13))
in ANSYS13-fluent, there are options for modeling wave (Airy, stocks,...) and free surface, but it takes times to realize. however, in this way you can simulate completely your problem.
my firs your problem was like "picture 1111" (likes your problem) and my result after modeling in new version of fluent is like "picture 2222" (that wave does not damp)

Also this link can help you for modeling wave in ansys-fluent: http://www.cfd-online.com/Forums/flu...-modeling.html

I hope my suggestion will be helpful.

[Jenn]

Dear saeed,

Would you please also share your experience with inlet and outlet settings?

Thanks a lot.
Jenn

[SeaYiTheng]

Dear Saeed

Hi I am trying to simulate waves too but it dampens out a lot over distance. I am using ANSYS version 16.2. Are you using UDF to generate waves? Can you share with me your UDF code? yithengs@gmail.com
Your help is very very much appreciated

Regards,
Yitheng

[wester]

Dear Arun,

I think your result doesn't looks like a wave damping issue. It looks like that there was not enough simulation time for getting the fully developed wave - the initial wave just starts propagating into the calm water area. It might be better to apply the initialization option to fill the whole domain with the wave.

If you don't want a current-wave interaction, start with the zero current/wind velocity.

Also, please check the wave period and length again. It doesn't match.

Regards,
Don

[SeaYiTheng]

Dear Wester

Attached is the screenshot of the wave I generated, T=1 sec, A = 0.05m using UDF code. As you can see the damping issue is very serious where the wave just disappeared over the distance. Could you please share with me how could I solve the damping issues in my case?
Appreciate your help

Regards,
Yitheng

[wester]

Hello SeaTiTheng,

Sorry for the late reply. I can't make sure what was the main damping source just based on the attached image. Frequently, the reflected wave on the outlet boundary might be one of the reasons. Usually, if possible, adding an extra domain (space) is recommended to resolve this wave reflection issue. Also, gradual changes in meshing size and additional numerical damping (or smoothing) is useful to suppress the unwanted wave reflections.

Cheers,
Dong

[SeaYiTheng]

Hi Wester

Thanks for the reply! But i guess reflection might not be the issue here as what I am showing in the picture is the the first three waves that are generated from the moving wall on the right. The first three waves have not reached the left wall yet for reflection to occur i think. As you can see, the first wave is moving from the right to the left and the wave height reduces a lot compared to the waves on the right. Do you have any idea why this happens?
Do let me know if you need any more information on my setup. Appreciate your help

Regards,
Yitheng

[wester]

Hi SeaYiTheng,

What's the physical time of the attached image? You have to wait a sufficient time for the fully developed wave field. Assuming a deep water wave, (actually your case looks like an intermediate depth), phase velocity is 1.56 m/s, and group velocity is 0.78 m/s. So you can figure it out how much time needs for the fully developed wave field.

Also did you check if your wave input is valid? It seems like that the your wave input is not appropriate to obtain a very sinusoidal linear wave - not enough water depth and too steep wave profile.

Thanks,
Dong

[miladzabihi]

hello, I hope your problem has been solved. however, I had the same problem, have you used turbulence models? damping may occurs due to turbulence models

[miladzabihi]

Originally Posted by SeaYiTheng

Hi Wester

Thanks for the reply! But i guess reflection might not be the issue here as what I am showing in the picture is the the first three waves that are generated from the moving wall on the right. The first three waves have not reached the left wall yet for reflection to occur i think. As you can see, the first wave is moving from the right to the left and the wave height reduces a lot compared to the waves on the right. Do you have any idea why this happens?
Do let me know if you need any more information on my setup. Appreciate your help

Regards,
Yitheng

hello, I hope your problem has been solved. however, I had the same problem, have you used turbulence models? damping may occurs due to turbulence models

[ping]

you can use laminar flow for simple wave modelling but this is not normally the issue - the key is to get the mesh parameters and time step correct within the wave and the free surface - the user guide is very specific about this so apply these rules carefully - Simulating Physics > Modeling Multiphase Flow > Modeling VOF Waves > VOF Waves Guidelines

[miladzabihi]

Originally Posted by ping

you can use laminar flow for simple wave modelling but this is not normally the issue - the key is to get the mesh parameters and time step correct within the wave and the free surface - the user guide is very specific about this so apply these rules carefully - Simulating Physics > Modeling Multiphase Flow > Modeling VOF Waves > VOF Waves Guidelines

thanks for your prompt reply. actually i am using ansys fluent. my project is to study wave- structure hydrodynamic. I use implicit solver where courant number is not important. the problem is that changing mesh or time step sometimes cause wave damping in an identical case, especially when I put a structure in wave propagation direction. do we have any criteria for courant number? any help will be appreciated
Thanks

[ping]

well thanks for wasting our time here and please have this discussion moved to the fluent stream

[zaoui]

I am doing a 2D simulation for wave propagation and my problem is that for the same wave parameters and the same setting the propagation in ANSYS-CFX is not the same as in ANSYS-FLUENT and it seems that in Fluent the wave decay .
I need your help please
u are welcome for more explanations

[ping]

well you have come to the right forum to get advice on how to do waves well but take a step backwards and start using the code more suited for any marine related model ie star

[morelix]

Use the 2. order implicit time discretization. The first order implicit discretization causes the effect of wave damping. (At least in Star-CCM+)