CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Why icoFoam solver results are not true for cavity (10000>Re>5000) ? (http://www.cfd-online.com/Forums/openfoam/78991-why-icofoam-solver-results-not-true-cavity-10000-re-5000-a.html)

maysmech August 9, 2010 11:57

Why icoFoam solver results are not true for cavity (10000>Re>5000) ?
 
Dear Foamers,
i used icoFoam solver for cavity. when the reynolds number is below 5000 the results are good. but for reynolds 5000 and 10000 results are different from Ghia benchmark. i promoted orders of discretisations in fvSchemes but results were same.
it is wondering because for reynolds below Re=10000 the cavity case is laminar and icoFoam should leads to true results.
:confused:WHAT IS THE PROBLEM?

stevenvanharen August 10, 2010 10:44

Hi maysam,

I am assuming you are referring to the lid-driven cavity flow.

i think both Reynolds number will not result in steady laminar flow. The OpenFoam user guide switches to pisoFoam for Re = 10^4. Botella and Peyret found unsteady behaviour at least for Re=9000.

What is your source for assuming laminar flow for Re < 10^4?

maysmech August 10, 2010 15:25

???
 
I examined cavity lid driven with pisoFoam RAS but results are same as icoFoam. for Re= 10000 and 5000 results are far from Ghia benchmark:confused:

stevenvanharen August 11, 2010 04:48

Ok, I will look at the Ghia paper this afternoon.

In the mean time, in what way do your results differ from the Ghia paper? In what way are velocity plots and pressure plots different?

maysmech August 11, 2010 05:02

Results for Re=10000.
velocity diagram over horizontal and vertical centreline.
U=1, D=1, nu=10^-4, time 100 sec


[IMG]file:///home/maysam/Desktop/U.gif[/IMG]http://www.imageupload.org/image.php...9_4C626678&gif

stevenvanharen August 11, 2010 08:57

Ok, I am not a 100 percent sure about what it is but I have some thoughts:

- Ghai et al use upwinding, are you using upwinding too in icoFoam? Could it be that your numerical diffusion is less strong than theirs? The fact that your velocity profile is less smooth suggests this.
- the fact that you use upwinding could explain the laminar solution for Re=10000.
- numerical diffusion is less dominant at low Reynolds numbers, therefore your error increases for large Reynolds number
- I suggest you use the paper by Botella & Peyret (1998), their method is much more accurate (spectral) and they also compare to Ghai et. al., unfortunately only up to Re = 1000.

Hope this helps!

maysmech August 12, 2010 04:10

Quote:

Originally Posted by stevenvanharen (Post 271145)
Ok, I am not a 100 percent sure about what it is but I have some thoughts:

- Ghai et al use upwinding, are you using upwinding too in icoFoam? Could it be that your numerical diffusion is less strong than theirs? The fact that your velocity profile is less smooth suggests this.
- the fact that you use upwinding could explain the laminar solution for Re=10000.
- numerical diffusion is less dominant at low Reynolds numbers, therefore your error increases for large Reynolds number
- I suggest you use the paper by Botella & Peyret (1998), their method is much more accurate (spectral) and they also compare to Ghai et. al., unfortunately only up to Re = 1000.

Hope this helps!

Dear Steven,
Thanks for your suggestions.
i examined icoFoam for Re=100, 400 and 1000 and there was no difference between them and Ghia et al.
but there was problem in 5000 and 10000 and it is solved by considering two things::)
- I should use higher order discretisation method i used vanleer.
- I shouldn't use initial value u=0 for all domain. i used steady state velocity and pressure of Re=1000 for Re= 5000 and also used steady satate values of Re=5000 for 0 folder of 10000. i think it is an important work for high reynolds problems.:cool:
Best wishes,
Maysam


http://www.imageupload.org/image.php...A_4C63A958&gif

stevenvanharen August 12, 2010 16:12

ok, first of all congratulations on solving the problem!

But your solution should be independent of the initial velocity field!

In the previous simulation which yielded the erroneous results how did you stop the simulation? A simulation with a higher Reynolds number should take longer to converge to a steady state solution (in physical time).

maysmech August 12, 2010 16:42

for Re=1000 after 20 sec the problem became steady and i let 50 sec for 5000 and 100sec for 10000. i thought the time was sufficient to become steady because i didn't see any changes in several last time steps by eye.
maybe it was not enough i will try it with more time because a sudden shock in high reynolds leads to late steady and putting steady state values of lower Re to 0 values of higher Re makes less run time.


All times are GMT -4. The time now is 15:28.