[caohan]

Hi, all

I got a question, does fluent can predict the transition point when doing a 2D aerofoil or 3D blade test. if not, can I manually set that point? and how can I set this point.

Thanks
Regrads
Han

[jack1980]

Fluent won't predict the transition point.

To set it manually, in the mesh generator you will have to split your domain into two zones. Then in Fluent, you can force one zone to be laminar. Let me know if you can figure it out, otherwise I'll give you a step-by-step explanation.

Good luck!

[caohan]

Originally Posted by jack1980

Fluent won't predict the transition point.

To set it manually, in the mesh generator you will have to split your domain into two zones. Then in Fluent, you can force one zone to be laminar. Let me know if you can figure it out, otherwise I'll give you a step-by-step explanation.

Good luck!

Hi jack

Thank you for your explanation, I think maybe I can figure it out a little, did you mean I need to split the domain into two parts which are left domain and right domrian？ if it is, how to set the boundary condition in Gambit? Can I ask a further question, if the model is 3D, can I use the same way to set the tranisiation point? hope you can help me

Han

[jack1980]

Hi, that's right, split the domain in left and right part. The interface will be your transition point. In Gambit, you have two buttons to set boundary conditions. The left is for surfaces (this is the 'usual' one), the right is for volumes. Just give the zones appropriate names, like 'laminar' and 'turbulent'. Then, in Fluent, you can force the 'laminar' zone to be Laminar. This also works in 3D.

Good luck with your simulations!

[caohan]

Originally Posted by jack1980

Hi, that's right, split the domain in left and right part. The interface will be your transition point. In Gambit, you have two buttons to set boundary conditions. The left is for surfaces (this is the 'usual' one), the right is for volumes. Just give the zones appropriate names, like 'laminar' and 'turbulent'. Then, in Fluent, you can force the 'laminar' zone to be Laminar. This also works in 3D.

Good luck with your simulations!

Thanks for your explation, I would try that method, by the way. do you know how to mesh a single blade with Hex in Gambit, just like the pic that I post. It can be meshed with Hex in cooper way when I remove the blade, but when I subtract the volume with single blade, the only meshing method is using Tgrid. Did you meet that problem before?

Han

[jack1980]

There's no picture I'm afraid. But for Hex-Cooper, you are making a structured grid? You could make a "block structured grid". Look for some examples in Google - images.

[caohan]

Originally Posted by jack1980

There's no picture I'm afraid. But for Hex-Cooper, you are making a structured grid? You could make a "block structured grid". Look for some examples in Google - images.

OK , I would try that, thank you

[DoHander]

Hello,

if you use Fluent 12 you can use a turbulence model that also models the transition (you 2 choices, one of them is the model of Menter).

If you use an older version you must split your mesh in a few blocks in order to be able to select one of them as laminar regions.

For external aerodynamics you can simply split your mesh using 2 vertical lines (one for each side of your 2D airfoil), see this article for an example:

Transition-Flow-Occurrence Estimation: A new method, Journal of Aircraft 2010, Vol. 47, no 2 by P.-D Silisteanu and R.M. Botez

If you are thinking at a flow through a turbine you must use a more elaborate method to define your laminar regions (each region must have a height of about the thickness of the laminar boundary layer and so on ...). I don't think it is practical to use Fluent 6.x for such calculation. I've seen such a modelization in a recent AIAA paper but I don't remember the title now.

Do

[galtmann]

I'm trying to model forced transition with a trip strip on a 2D airfoil in fluent 12.1. I did not think about trying to split the entire domain into two zones, so I'll try that, but the original way I wanted to model it was with the transition SST model in fluent 12. In this model, they supply an area to insert a user defined function (UDF) to fix the point of transition. The only problem is the example UDF they supply is as follows:


#include "udf.h"

DEFINE_TRANS_FLENGTH(user_Flength, c, t)
{
real Flength = 31.468;

return Flength;
}



I am not sure what this does. I origionally thought it was a fixed distance from the stagnation point, but I applied the distance of the trip strip to Flength, and it did not change the solution at all. Am I doing something wrong?

Thanks for your input!

[galtmann]

Yea... I just tried running a laminar zone before the trip strip, and then turbulent everywhere else and I did not match my experimental data; the solution was the same as the baseline case where the entire flow is turbulent. Anyone have any ideas???

[DoHander]

In order to understand why you can't obtain any solution improvement please give me some names and numbers: your M, Re and alpha, the kind of airfoil, sources of experimental data, the position of the transition "points" on both faces of your airfoil.

Also I need to know what turbulence model you have used and what was your y+, type of your boundary conditions etc ...

Do

[galtmann]

Originally Posted by DoHander

In order to understand why you can't obtain any solution improvement please give me some names and numbers: your M, Re and alpha, the kind of airfoil, sources of experimental data, the position of the transition "points" on both faces of your airfoil.

Also I need to know what turbulence model you have used and what was your y+, type of your boundary conditions etc ...

Do

Mach: 0.07
Re: 1.08x10^6
Alpha: for this case, 0 degrees
Airfoil: NACA0036 to simulate bluff bodies
Turbulence Model: Both k-w SST, and Transition SST found in Fluent 12.1
y+: all less than 1
Boundary Conditions: Walls, with wind tunnel walls modeled with y+=1, then velocity inlet, pressure outlet (pressure based solver)

I am taking pressure data from several AIAA conference papers (2003-3516,2006-322) along with wind tunnel data I'm taking at our university wind tunnel. All data is surface pressure data taken with 34 pressure ports.

All published experimental data has trip strips forcing transition at 5% of the chord, with flow visualization to confirm this. For my data, I took both forced and natural transition data. Even though a NACA 0036 is a bluff body with massive separation at higher angles of attack, at 0 degrees the CFD k-w model can predict the separation and pressure distributions perfectly for natural transition. When the trips strips are added at 0 degrees, I am seeing earlier separation; so this is what I'm trying to model.

If you need addition info please let me know.

Thanks for your help, I'm really stuck with this one.

[DoHander]

Can you give me the names of AIAA articles ?

Do

[DoHander]

However if you trip the transition at 5% of your airfoil (0.05 for a chord of 1 meter) I suppose you will see no difference if you use a transition model or not (practically your airfoil is 95% in turbulent zone).

Probably you should open a new thread asking about a proper turbulence model for separated flow and keep your entire domain as a turbulent one.

Do

[galtmann]

2003-3516 "Active Separation Control - Measurements and Computations
for a NACA 0036 Airfoil"
2006-322 "Control of Massive Separation on A Thick-Airfoil Wing: A Computational and Experimental Study"

Maybe you're right about the entire region being turbulent. But what gets me is the fact that without the trip strips I can model the flow at 0 degrees, but when the trip strips are added, the separation location point changes (moves aft), which says to me that I have to model the early transition. After researching this a little bit, I think that what is happening is the early transition is creating a taller boundary layer which causes the boundary layer to separate earlier. Any thoughts?

[kdrbrk]

Originally Posted by DoHander

Hello,

if you use Fluent 12 you can use a turbulence model that also models the transition (you 2 choices, one of them is the model of Menter).

If you use an older version you must split your mesh in a few blocks in order to be able to select one of them as laminar regions.

For external aerodynamics you can simply split your mesh using 2 vertical lines (one for each side of your 2D airfoil), see this article for an example:

Transition-Flow-Occurrence Estimation: A new method, Journal of Aircraft 2010, Vol. 47, no 2 by P.-D Silisteanu and R.M. Botez

If you are thinking at a flow through a turbine you must use a more elaborate method to define your laminar regions (each region must have a height of about the thickness of the laminar boundary layer and so on ...). I don't think it is practical to use Fluent 6.x for such calculation. I've seen such a modelization in a recent AIAA paper but I don't remember the title now.

Do

Do,
For 3D external flows with NACA 6 series airfoils (almost %60 laminar) which transition model would you suggest?
And can I trust the results?

Regards
Kadir

[DoHander]

@kdrbrk

I would try with the two transition models from Fluent 12 for 3D. In order to check the models you can do a 3D calculation on very long wing (or a wing between two walls) and compare the Fluent results with experimental 2D data.

Do

[kdrbrk]

I just wanted to know with a shortcut if you had any experience, but ok I will try.

[DoHander]

Actually I've used the model of Walters and Cokljat in Fluent 12 for a 3d wing, but I didn't have the chance to compare the results with experimental data.

What I've compared with experimental data was the method presented in the article cited above for 2D calculations.

So you see why I can't give you a clear recommendation for 3D calculation, this is why I've suggested to test the transition models from Fluent with some experimental data (if you have any).

Do

[kdrbrk]

Thanks Do.

Currently I don't have any experimental data but I will look for some.