Hi to all

I have seen at www.turbulentflow.com some interesting information on V2F viscous model. As I am working with bluff bodies, I think this model might be interesting. But I don´t know anything about it. How can it be used? Is it an upgrade for regular Fluent 6.0 or 6.1????

I am interested as the results seem to be better than regular K-e models.

Anyone can help?

Miguel

I used the V2F model on a bluff body simulation and got some improvement in the results, but not a huge difference over a k-e realizable. I noticed about a 5-10% increase in time/iteration (running 3D compressible with V2F versus same with k-e realizable) plus about 5% more iterations to convergence, and only about a 2% improvement in the forces compared to wind tunnel results (I was only off about 10% with the k-e model, so we ended up dropping V2F for improved convergence times). The main difference I noticed was an improvment on the location of the separation point, and a slight improvement on the pressure distribution along the surface in the separated region.

From what I remember, they were claiming less sensitivity to y+ values, but my results weren't confirming that. Could be something I was missing in setup, but in 2 to 3 month programs, you don't get a lot of time to narrow down the intricacies of a new model... just gotta go with what you know.

It's not something Fluent gives out, it's an additional charge. I know the add-on works for anything after Fluent 6.1, and I think it works for 6.0 as well. You'll have to contact your Fluent Rep for pricing and what-not. You might be able to get a trial license for the V2F model... it's worth asking about at least if you're interested.

Hope this helps, and goodluck, Jason

Thanks Jason

I will have a go at it. As I am trying to model bluff bodies with not very good result I will thank you if you could answer some questions.

At the moment I am working in 2d.I have done quite a good mesh (skew<0.04) and I have tried some viscous models.

-Spalart allmaras: works well with long bluff bodies (length=4R; width=R) but oscilates with short ones(lenght=2R)

-K-e standard with enhanced wall treatment: works average with long bluff bodies (length=4R; width=R) and average with short ones(lenght=2R)

-K-e realizable with enhanced wall treatment: diverges with long bluff bodies

-K-e RNG with enhanced wall treatment: diverges with long bluff bodies

All have been tried with the same mesh with an Y+<1, a velocity inlet of 5m/s and a pressure outlet of 0, with operating pressure of 0.

Which do you think is the most suitable model for 2d? and for 3d?

Thanks:

Miguel

I had excelent results with K-e Realizable in 2D and 3D, but I used 30 < y+ < 200. This keeps you out of the laminar region of the BL. If you do near wall treatments with the k-e realizable, then you need y+ < 1, but otherwise I recommend staying between 30 and 200.

At 5m/s are you sure you're even turbulent? Quick hand calc says that unless you've got about a 1.5m diameter, you're below the critical reynolds number, and a Laminar model may be a better model for you.

Divergence can usually be contolled by your solver settings. At such a low velocity, use the segregated solver... I recommend setting your pressure URF to 0.5 and your momentum URF to 0.4. Also, set your limits... I recommend setting your absolute pressure limits to static plus or minus three times your dynamic pressure (no matter what your airspeed is). For such a low velocity I would put my temperature limits to 40 degrees above and below ambient (I usually guess the temperature variation and do about 5x to 10x that for the limits). Turn off the turbulence equation and run it first order for 100-200 iterations, then turn turbulence back on and run it first order to convergence. Switch to second order (on everything but turbulence and pressure-velocity coupling) and run to convergence.

Hope this helps, and goodluck, Jason

Jason:

The bluff body has a width of 1m, which makes Re=3,4E5. I believe we are already in a turbulent phase.

I followed your recommendations step by step and it has diverged and created great turbulence.

I might be in some kind of error but I don´t understand a thing about it because before diverging, the Cd values where very low (errors of 50%).

Any other help?

Many, many thanks

Miguel

How many iterations into the solution until it diverges? What solver settings are you using when it diverges?

Jason

let´s see:

-I did what you told me; i.e.Pressure URF=0.5 and Momentum=0,4 I turned off the turbulence equation, run 200 iterations. I turned the equation on and run about 1000 iterations until almost-converged. Then I switched to 2nd order pressure and momentum.

It started Diverging about 2600 iterations

Now about the solver settings:

the settings are: -segregated, implicit, 2D, steady, absolute

-About the viscous model: K-e realizable with standard wall functions; c2=1.9; TKE=1; TDR=1,2 Turbulent viscosity=none

-About the mesh; skew<0,05 velocity inlet and pressure outlet. The bluff body is something like a bullet and the mesh keeps on for 30 times the bullet lenght behind.

I don´t know why but with K-e standard it converged but to a value of Cd around 0,4 whilst the air tunnel value is or ariund Cd=0,7

Any clue?

Thanks; Miguel

As for the Cd value, two things to consider...

Drag on a cylinder doesn't seem to drop until a RNL of about 3-4(10^5) based on the diameter (Hoerner, Fluid-Dynamic Drag). You could be in the transition region, which is notoriously difficult to solve. You could try a laminar model to "bound" your solution.

Also, double check your reference values (very common problem).

As for the divergence, you'll have to really look at the solution when it diverges to see where the issue is happening. If you save a case and data just after it diverges and send it to me, I'll take a look at it when I get a chance and let you know what I find and what to look for in the future.

Hope this helps, and goodluck, Jason

thanks Jason

I will work on it and I wills end it ASAP

Thanks again

Miguel

[hamide]

hi all
i want to simulate turbulent flow in a 2D channel (2*40cm) by v2f model.
i set it as follow:
-i try to use fine mesh near the wall, (y+<=1)
-B.C : velocity inlet, v=5 m/s , and define functions for v,k,epsilon and v2.(to be fully developed from beginning of channel)
outFlow for end of the channel
nosleep fo walls.
-second order upwind to solve equations.


but unfortunately i can't valid my results!!!!!! for example i can't find u+ vs y+ graph correctly!!! and also v'+ vs y+ and k+ vs y+ near the wall!!!!(1<y+<100)
i don't know what the problem is!!!!
is there any one help me to handle this problem.