Hi! I am doing free surface
 

Hi!

I am doing free surface analyses for a NACA profile using rasInterFoam. I have a domain (3D) with only one common inlet patch for both water and air. The inlet condition for gamma is zeroGradient and so is the outlet condition as well. Is this proper or do rasInterFoam need two separate inlet patches for water and air respectively or perhaps some other inlet condition? Pd at the inlet is also set to zeroGradient just as at the outlet.

The reason I am asking is because the results (at T=0.4s) looks a bit strange with a very sharp wave that seams unrealistic as the flow velocity is set to 2 m/s.

Best Regards!
/Hardy

Adding a picture of the domain
 

Adding a picture of the domain with iso-surface of gamma= 0.5!

http://www.cfd-online.com/OpenFOAM_D...your_image.gif

/Hardy

Here we go again! http://ww
 

Here we go again!

http://www.cfd-online.com/OpenFOAM_D...ges/1/7502.jpg

Hi Hardy Nice picture, thou
 

Hi Hardy

Nice picture, though I am not familiar with the NACA profile, so could you please give a couple of details on the setup.

Best regards,

Niels

Hello Niels and thanks for sho
 

Hello Niels and thanks for showing interest in my problem!

Inlet (one common inlet for both phases) and outlet are as described in my first post. The bottom and naca-profile are walls. The sides are symmetryplanes. The top surface is atmosphere taken from the rasInterFoam dambreak tutorial. Schemes and other settings are from the same tutorial. I use the k-epsilon turbulence model.

Are there any other specific details you would like to know?

/Hardy

Hi Hardy Actually I was mor
 

Hi Hardy

Actually I was more after the physical setup, i.e. a description of the problem you are investigating numerically. Though I might be able to help you anyway.

First of all you are not writting what your outlet on U is, but I suspect you have used dU/dn=0? If that is the case you will experience problems, so I would use pd=0 at the outlet.

The wave looks a bit strange, but have you initialized the flow velocities inside the domain to be the same velocity as at the boundary? If not a setup of some sort should be expected.

Hope is helps,

Niels

Hi again! The aim with my a
 

Hi again!

The aim with my analysis is to evaluate the wave pattern for this naca profile and compare with experiments and other CFD-results.

Yes, U at outlet is set to zeroGradient, do you have some other suggestion? For pd I have tried both pd=0 and zeroGradient.

I will try to do some more clever initialisation!

Thank You!
/Hardy

Hi You could try to make a
 

Hi

You could try to make a soft start, i.e. multiply your velocity field at the inlet by a factor f(t) in [0,1], where f(0) = 0 and f(hotstart_end) = 1. This would slowly ramp up your system and you might overcome the wave problem.
f(t) = sin(omega * t) could be a nice way to start. This imply that you have to use a timeVaryingFixed boundary condition. Search the forum, because there is a discussion on such boundary conditions.

Best regards

Niels

Hardy, you may take inspirati
 

Hardy,
you may take inspiration from the boundary conditions here attached
http://www.cfd-online.com/OpenFOAM_D...s/mime_zip.gif BC.zip
These conditions are the same included by Eric Paterson in the following thread :
http://www.cfd-online.com/OpenFOAM_D...tml?1203948011
I found them very robust in free surface flows.
I suggest to take a look at the whole wigley case of Eric for a proper setup.

Regards,
Michele

Thank you for helping me out!
 

Thank you for helping me out!

I will take a good look into Eric´s case!!

So I need to separate my common inlet into one inlet for each phase?!?!

/Hardy

Yes, I usually prefer this sol
 

Yes, I usually prefer this solution.

Otherwise you should specify inlet gamma on a face-by-face basis in the inlet patch.

Michele

Hi again! I have now implem
 

Hi again!

I have now implemented separate inlet patches and a set-up as described by Paterson´s Wigley case. (I use k-epsilon turbulence modelling.)

However I am experiencing difficulties as the pd-pressure goes to high values both positive and negative. The extreme pressures are positioned on the mast´s trailing edge at the hight of the free surface, see figure. The time step is decreasing during the simulation, in order to meet maxCo set to 0.2 I guess.

Does anyone have any suggestion how I can overcome this situation??

Best Regards! /Hardy

http://www.cfd-online.com/OpenFOAM_D...ges/1/7599.jpg

One more figure! http://www
 

One more figure!

http://www.cfd-online.com/OpenFOAM_D...ges/1/7601.jpg

Hardy, It is hard to tell w
 

Hardy,

It is hard to tell what is going on from the images. If you upload your case to http://idisk.mac.com/egpaterson-Public I'll take a look and see if there is any obvious problem with your setup.

Also, we went through a validation exercise last year for a surface-piercing NACA 0024. Animations and images are supposed to be on our website http://www.arl.psu.edu/capabilities/fsm_compmech.html, however, I've been too busy to write up that section. I can post them on mac.com account if you would like.


Eric

Hello! I have now uploaded
 

Hello!

I have now uploaded naca.tar.gz, please have a look :-)

Are you perhaps refering to the NACA0024 experiments made by the university of Iowa. My organization made of validation of this using Fluent a couple of years ago. My present objective is to again validate this, now by using openFOAM. Looking forward to see your results when you have them on your website!!

Thank You! /Hardy

Yes, I am referring to the IIH
 

Yes, I am referring to the IIHR experiments done by Metcalf, Longo, and Stern. You can get some of the data from their website http://www.iihr.uiowa.edu/~shiphydro...ata_naca24.htm. Since I did my PhD at IIHR in the early 90's, and was the original developer of CFDSHIP-IOWA (a free-surface RANS solver), I know the experiment and previous CFD simulations well.

Eric

Hello Eric, I am looking fo
 

Hello Eric,

I am looking for torture techniques for one of my students at Uni Zagreb (final project). Looking at experimental data and esthetic beauty of the flow, I would like to work with the student to study the piercing airfoil case in detail. Would you consider donating the mesh for OpenFOAM simulation in return for access to all results?

Please let me know,

Hrv