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

Please help with separation bubble

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 16, 2002, 13:12
Default Please help with separation bubble
  #1
Nael
Guest
 
Posts: n/a
Hello everyone,

I have to look at laminar separation with bubble formation on an aerofoil. (FLUENT 5)

It is 2D and I am working on Viscous > Laminar -Is this the right choice?

I have simulated the flow at 0, 2, 4 ... 15 degrees of incidence and the flow stays attached on the whole range of incidence, which is obviously not normal- it's as if there was no viscous effect.

I'm desesperate for help.

Thanks
  Reply With Quote

Old   March 18, 2002, 18:46
Default Re: Please help with separation bubble
  #2
Rob
Guest
 
Posts: n/a
Nael,

I have done a bit of 2-D transonic airfoil case studies. I had the same results as you at first. The only way I was able to accurately pick up on a separation point, and laminar separation bubble, was by splitting the flow over your aifoil in to a laminar and turbulent region. If you have an idea of where your flow transitions from laminar to turbulent that is where you would split it. Then in setting up your boundary conditions you would set the first region as a laminar zone. And then the second region, your turbulent region would use whatever viscous model you picked. I ended up with good results by using the standard k-e model with the 2-zonal wall treatment. It picks up a good cp and cf plot over the airfoil that way.

I hope this helps some.

Rob
  Reply With Quote

Old   March 19, 2002, 03:12
Default Re: Please help with separation bubble
  #3
Nael
Guest
 
Posts: n/a
Thanks a lot Rob,

How do you split the flow over the airfoil into laminar/turbulent region? Do you create to inlets - the second one being at an estimate of the transition region?

Also, how did you find an estimate for the distance where the transition occurs?

Thanks again for your help.
  Reply With Quote

Old   March 21, 2002, 15:37
Default Re: Please help with separation bubble
  #4
Rob
Guest
 
Posts: n/a
Nael,

The way to split your flow field into two regions (laminar/turbulent) is in your grid software. In Gambit what you do is split the field on the top of the airfoil and the bottom of the airfoil. Then at the split you define it as an interior boundary condition. This way Fluent knows it is not an inlet or an outlet, just an interior surface. Then when you read the grid into fluent under boudary conditions you must set the laminar region of your fluid to a laminar zone.

As far as finding out where your transition point should occur, I am not sure what is the best way to do that. What I did to find that point is to run the airfoil case on a 2-d panel code such as XFOIL or MSES. Depending on your free stream mach number one code might be more accurate then the other, however both should work well enough to predict transition. XFOIL is freely available on the net by going to http://raphael.mit.edu/xfoil/ while MSES is not. MSES works better in transonic fow however. This is a good way to validate your results obtained from FLUENT also.

If you have any other questionsor need me to be more specific go ahead and email me or just keep posting and I will do my best to answer any questions.

Good luck...Rob
  Reply With Quote

Old   March 21, 2002, 16:51
Default Re: Please help with separation bubble
  #5
Nael
Guest
 
Posts: n/a
Rob,

Thanks a million, I really appreciate your help.

My project is on FLUENT only; I cannot use another software. I am going to try to understand your method and come back to you with a few questions.

So you're saying I should use viscous > laminar for the first region, then use k-epsilon for the second region?

Thanks again mate.

  Reply With Quote

Old   March 22, 2002, 03:50
Default Re: Please help with separation bubble
  #6
Rob
Guest
 
Posts: n/a
Nael,

You pick viscous -> k-epsilon as your turbulent model. Then when you go to set your boundary conditions, you specify your first fluid region as a laminar zone. There will be a box for you to click on and activiate the zone as a laminar zone in the boundary condition panel. I am not at my computer with FLUENT on it so I can not give you exact locations at the moment, but I would be more then happy to if you want. Again hope this helps some.

I am not sure how you could accurately predict transition without the use of another code. I would guess that there would have to be something in literature out there somewhere.

Rob

  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
Solver for gas bubble separation in T-junction endremossige Main CFD Forum 0 February 22, 2010 10:44
Laminar bubble separation Gilles CFX 1 July 24, 2008 21:57
Separation bubble, hypersonic compression corner ben akih CFX 3 December 10, 2006 17:33
Laminar separation bubble Axilleas Tsompanos FLUENT 5 August 6, 2004 12:24
separation bubble Celia Main CFD Forum 0 July 10, 2004 23:17


All times are GMT -4. The time now is 16:27.