CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Submerged fin, Convergence problem (https://www.cfd-online.com/Forums/fluent/64848-submerged-fin-convergence-problem.html)

supermouniette May 26, 2009 12:48

Submerged fin, Convergence problem
 
Hello everybody!

I have a convergence problem and it is making me crazy! I am going to explain the situation as clearly as possible.

I have to model a fin completely immersed into water to determine the lift, drag and moment coefficient.

Here are the flow characteristics:
Speed : 1 m/s
Temperature : 277.15 (3C)
Reynolds number : 7900
Rho : 1034.53 kg/m3
Viscosity : 0.00167 Pa/s

Fin angle of attack= 0

This is how I use Fluent:
  • k-e model standard, implicit
  • steady
  • BC inlet : velocity inlet(1m/s), turbulent intensity(0.1%), turbulent viscosity ration(5)
  • BC outlet : pressure outlet (1.51e7 Pa), turbutlent intensity(0.01%), turbulent visosity ratio(10)
  • Pressure discretization: "1st order" for the first 500 iterations then "Linear"
  • Momentum, Turbulent kinetic energy and Turbulent dissipation rate discretization : "1st order" for the first 500 iterations then "Second order Upwind"
  • Pressure-velocity coupling : SIMPLE
  • Under relaxation factors set as default
I monitor residuals, CL, Cd and Cm.

First problem : I have the following error "turbulent viscosity limited to 1e5 in 1 cell". Is it an important error? I would say no because it is only in 1 cell, but give me your opinion please.

Second problem : CL, Cd and Cm don't stop oscillating! There is no convergence after 5,000 iterations. I tried to decrease the under relaxation factors but it didn't help to converge.

Third problem : the continuity residuals remain at 1. But it is not the major problem! the second one is!!

I really don't know what to do to solve these problems! I am not used to use FLUENT for "water problems", so maybe I forgot something.

Help me, please!!:) thank you in advance

Julie

Ralf Schmidt May 27, 2009 03:45

Hi,

there might be something wrong with your grid....

check grid quality and yplus values at your walls....

For oscillation of the residuals and residuals, see
http://www.cfd-online.com/Forums/flu...cillation.html
and http://www.cfd-online.com/Forums/flu...tml#post127748


Best wishes
Ralf

Dimo May 27, 2009 05:33

What are the dimensions of your fin?

I might be wrong, but your Re is relatively low, so you might be in the laminar regime. I'd recommend you make a run with laminar, then try to move on to a turbulence model, it could help you with having an initial idea of what values to expect.

Also why are you setting pressure outlet to 1.51e7 Pa?

Hope it helps, please anyone feel free to correct me if I'm wrong so I can learn too.

Dimo

Ralf Schmidt May 27, 2009 06:05

Quote:

Originally Posted by Dimo (Post 217287)
What are the dimensions of your fin?

I might be wrong, but your Re is relatively low, so you might be in the laminar regime.

Dimo

How do you calculate your Re number?

supermouniette May 27, 2009 11:28

Quote:

Originally Posted by Ralf Schmidt (Post 217294)
How do you calculate your Re number?

I calculate my Reynolds number as follows:

Re= rho* V* L/ mu

rho=1034.53 kg/m3
V=1m/s
L= mean aerodynamic chord (I have a swept-wing)
mu= dynamic viscosity= 1.67e-3 Pa.s

and the result is 7940.

I am running a laminar simulation to have an idea of the values and to check wether it is my grid or my model that is wrong.

I'll keep you posted
Julie

supermouniette May 27, 2009 11:35

Quote:

Originally Posted by Dimo (Post 217287)
What are the dimensions of your fin?

I might be wrong, but your Re is relatively low, so you might be in the laminar regime. I'd recommend you make a run with laminar, then try to move on to a turbulence model, it could help you with having an initial idea of what values to expect.

Also why are you setting pressure outlet to 1.51e7 Pa?

Hope it helps, please anyone feel free to correct me if I'm wrong so I can learn too.

Dimo

Here are the dimensions of my fin:

root chord: 0.1515 m
tip chord: 0.136 m
wingspan : 0.2 m

I am setting pressure outlet at 1.51e7 Pa because my fin is at a depth of 1500 m. So, as the pressure is about 151 bars (1.51e7 Pa) at 1500 m, I set this value.

Please, tell me if I'm wrong to do that.

Julie

Dimo May 27, 2009 12:14

Ok, let us know how you get along. Are you modifying the pressure in the Operating Pressure tab?

Dimo

supermouniette May 28, 2009 16:17

Hi,

To answer your question Dimo, yes, I changed the Operating Pressure and set it to 0.


I ran a simulation with the laminar model with an angle of attack of 0 and the results were still oscillating! So, I decided to run a simulation with a higher angle (2) and it is working.

I also ran a simulation with the laminar model ,with a structured grid, at alpha=0 and it is also oscillating. But for alpha=2, the solution seem to converge (the simulation is not finished yet).

I wonder why there is a problem when alpha=0. This is the simplest case and there should not have any problems...
If you have any ideas, please, let me know.

I have one question: When are we certain that the solution is converged? At which precision a value is said stable? I mean, my solution looks like CL=3.25e-4 +/- 0.1e-4. Can I consider that it is converged? I hope my question is understandable!

Thanks for your help!
I'll let you know the results when I get back from holidays:cool:

Julie

supermouniette June 26, 2009 10:26

Hello everybody!

Actually, my boundary conditions were wrong...I set every faces with "Wall" except the inlet and the outlet, so it made my flow unsteady. Now that I have changed them everything is fine, no convergence problem anymore.

Thank you for helping me.

Bye:p

Dimo July 6, 2009 09:45

What B.C. did you change?

supermouniette July 6, 2009 10:47

1 Attachment(s)
Quote:

Originally Posted by Dimo (Post 221608)
What B.C. did you change?

My control volume is a 3D-rectangle with the fin attached to one vertical face. I made a drawing for you to understand clearly (the file is attached). So, when you look at the drawing, I set the green face with "pressure oulet", the yellow one with "symmetry" and the other faces are set with "velocity inlet".


I set those BC because with only the "wall" condition it seems like the fin is in a closed box, where the flow passes through it.


I hope my anwer is clear.

Bye

Julie[IMG]file:///C:/Users/julie/AppData/Local/Temp/moz-screenshot.jpg[/IMG]


All times are GMT -4. The time now is 05:08.