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

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

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.

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

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.

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