CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Inlet conditions rasInterFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 28, 2008, 08:35
Default Hi! I am doing free surface
  #1
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
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
hardy is offline   Reply With Quote

Old   April 29, 2008, 09:43
Default Adding a picture of the domain
  #2
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
Adding a picture of the domain with iso-surface of gamma= 0.5!



/Hardy
hardy is offline   Reply With Quote

Old   April 29, 2008, 10:28
Default Here we go again! http://ww
  #3
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
Here we go again!


hardy is offline   Reply With Quote

Old   April 29, 2008, 11:46
Default Hi Hardy Nice picture, thou
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,607
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is online now   Reply With Quote

Old   April 30, 2008, 04:09
Default Hello Niels and thanks for sho
  #5
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
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
hardy is offline   Reply With Quote

Old   April 30, 2008, 04:43
Default Hi Hardy Actually I was mor
  #6
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,607
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is online now   Reply With Quote

Old   April 30, 2008, 07:34
Default Hi again! The aim with my a
  #7
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
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
hardy is offline   Reply With Quote

Old   April 30, 2008, 08:11
Default Hi You could try to make a
  #8
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,607
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is online now   Reply With Quote

Old   April 30, 2008, 08:31
Default Hardy, you may take inspirati
  #9
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Hardy,
you may take inspiration from the boundary conditions here attached
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
michele is offline   Reply With Quote

Old   April 30, 2008, 10:15
Default Thank you for helping me out!
  #10
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
Thank you for helping me out!

I will take a good look into Ericīs case!!

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

/Hardy
hardy is offline   Reply With Quote

Old   April 30, 2008, 10:38
Default Yes, I usually prefer this sol
  #11
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Yes, I usually prefer this solution.

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

Michele
michele is offline   Reply With Quote

Old   May 8, 2008, 07:18
Default Hi again! I have now implem
  #12
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
Hi again!

I have now implemented separate inlet patches and a set-up as described by Patersonīs 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 mastīs 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


hardy is offline   Reply With Quote

Old   May 8, 2008, 07:20
Default One more figure! http://www
  #13
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
One more figure!


hardy is offline   Reply With Quote

Old   May 8, 2008, 08:40
Default Hardy, It is hard to tell w
  #14
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
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
egp is offline   Reply With Quote

Old   May 8, 2008, 11:53
Default Hello! I have now uploaded
  #15
New Member
 
Hardy
Join Date: Mar 2009
Location: Sweden
Posts: 19
Rep Power: 8
hardy is on a distinguished road
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
hardy is offline   Reply With Quote

Old   May 8, 2008, 12:10
Default Yes, I am referring to the IIH
  #16
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
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
egp is offline   Reply With Quote

Old   May 8, 2008, 13:35
Default Hello Eric, I am looking fo
  #17
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
Dependence Inlet conditions : k and eps PK FLUENT 0 July 19, 2006 08:52
RasInterFoam boundary conditions maritozzo OpenFOAM Running, Solving & CFD 0 December 13, 2005 13:15
Pressure Inlet Conditions Sangeon FLUENT 2 September 26, 2003 05:42
Two Conditions in the inlet. Lucio CFX 1 June 28, 2003 09:09
Help please:Inlet Boundary Conditions!!! David CFX 4 October 31, 2002 20:03


All times are GMT -4. The time now is 16:56.