good morning CFD specialists;

I have confused what model to use for low reynolds numbe r flow around the german low speed airfoil FX . I used K-omega and K epsilon modles but the drag was about 50 % dieffrent from EXPerimental (dated both at 1930 and 2004). results

I want the fluent set up model for low Re. number as 150,000 to 500,000. Is laminer flow ok? or Some turbulance modle is better?

M. Essuri

If you don't know the transition point on the airfoil, then the best approach I use in this case, is this one:

- structured mesh, y+=1, B-L growth ratio=1.05;

- SST-kw model, with "Transitional flow" option activated (to select low-Re SST-kw);

- PRESTO discretisation scheme for Pressure;

- MUSCL discretisation scheme for Momentum;

- Second Order for all other variables;

- SIMPLEC Pressure-Velocity coupling scheme (this allows you to use higher URFs, like 0.8 for both Pressure and Momentum, and default for the rest, for faster convergence)

This approach has given me a 16% error for NACA0012 drag at null incidence, and down to 4% for some subsonic aircraft configurations (be careful, the MUSCL scheme does not include a flux limiter, so theoretically you should not use it for transonic configurations, although I found it to work for lower incidence, under 5 deg). Surprisingly, for incident flow, the results might be even better (this depends on the case)!

But if you know the transition point, be sure to construct your grid in such way that you can assign different "Fluid Zone" continuum conditions to the areas left and right of the transition point. This way, in Fluent you will be able to select "Laminar Zone" option for the fluid zone left of the transition point. This way you will force transition at that point. Of course, the solver settings should remain the same as I already described.

One last thing: start with first order settings, ask 250 iterations, for example, and then switch to the above ones, to avoid any divergence possibility.

Try this, you will not be dissapointed.

Razvan

hi Razvan,

I am doing a flow over two cylinders, I consider that my flow changes from Re = 350, I want to make it completely an external flow, just the wall of the cylinder. And the fluid medium is air, i just have the diameter of the cylinder and the length of the opening. I want to make it a 2-D problem. I want just the vorticity contours for different Re values.

Though I am familiar with fluent but have never done a turbulence problem, and youre answer was very good and precise so I thought you might help!

Could you tell me how I should I do my problem. I was reading few turbulence modeling topics and I guess that I should use SA, k-e, k-w models, (1)am I right?, (2)and what other input conditions will I need? (3) and how should I make my grid, coz I have never dealt with Y+, (4)I dont understand what it is?

Can you guide me or show me some reference.

I got a same tutorial from fluent website but its a laminar flow and the grid is already made, and I dont know how to make such a grid. (5) Should I consider my problem steady or unsteady? Any help from you will be appreciated! Rekha

Hola cabro,

you have to use V2F turbulence model