
[Sponsors] 
May 29, 2012, 15:31 
funny

#22 
Super Moderator

I had problems in meshing same geomtry in ICEM, four months ago.
Meshing of road vehicle I was making one silly and small mistake in that blocking. Could some pointout , what was it? 

May 29, 2012, 15:45 

#23 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Did you have difficulties on convergence? I see that with ke realizable, all solution methods on second order and default solution controls, continuity residuals slowly diverge. But almost halving the values of relaxation seems to remain stable and slowly converge. With my previous mesh (2M elements but wall distance of 0.1 mm, orthogonal quality above 0.5) i got convergence in about 10k iterations and about 8 hours. Using the pseudo transient combined with fmg initialization surprisingly the solution converged in less than 500 iterations, in 1h30m. But now using this method leads to an immediate divergence


May 29, 2012, 15:49 

#25 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
I'm actually using far3. What do you suggest?


May 29, 2012, 15:54 

#27 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
What settings and turbulence model?


May 29, 2012, 15:56 

#28 
Super Moderator

using enhanced wall treatment, first order scheme for few hundred iterations and then switched to 2nd order. But he has already done this on tetra + prism for same geometry.


May 29, 2012, 16:00 

#29 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Ok with my settings as I wrote here above now seems to be ok. I just switched to coupled solver with pseudo transient to speed things up and it's working. When finished I try with enhanced wall treatment


May 29, 2012, 16:03 

#30 
Super Moderator

because if the mesh has low yplus and you are using wall function then you certainly will have the problem. use either EWT or scalable wall function to keep the things under control.


May 29, 2012, 17:45 

#31 
Senior Member

So, the mesh you posted initially (alenglaro) caused some problems. The residuals for z and x velocity were having oscilations and the whole thing was converging very slowly. Here is the picture of the residuals:
Afterwards I checked the contours of Cp on the body and the ground and it revealed some kind of a hole/break/error in the mesh right beneath the rear surface of the body: The Cp there was ~47 (and max should be ~1), reference values were set correctly so we concluded it was an error with the mesh. Using Far's 3rd mesh we've got perfect convergence after 400 iterations (I was away when I initially set 500 after switching to 2nd order discretization for momentum, k and epsilon).. here's a screenshot of the residuals: The settings used were: RKE turbulence model, Enhanced wall treatment with pressure gradient effects, Coupled solver with momentum, k and epsilon in First order for 3050 iterations, then switch to Second order on all 3 and iterate until converged. Courant was set to 50, Explicit relaxations were set to 0.4 and only turbulent viscosity under relaxation was decreased to 0.8 for the First order iterations, then it was brought up to 0.95 for Second order. Here are the Cd and Cl convergence files. To reach full convergence, it took about ~56 minutes (8.23 sec per iteration). 

May 29, 2012, 17:57 

#32 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Thank you! This helps me a lot. Two questions. How can you set the courant number for pressure based steady solver? Coupled method is available only for pressure based. Did you use pseudo transient? Thanks again


May 29, 2012, 17:59 

#33 
Senior Member

No, I didn't use pseudo transient. Regular steady state and then Coupled instead of SIMPLE, Courant number is there under solution controls (i used 50 which is what I use for tetra meshes of lower quality/higher skewness) but in the end it only affects the convergence process.. end result is always the same, regardless of the courant/relaxation factors..


May 29, 2012, 22:24 

#34  
Super Moderator

Quote:


May 30, 2012, 11:21 

#35 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Ok I run a simulation with your settings and got convergence in 250 iterations, with residuals below 10^5. But cd is stable at 0.289. What's are your BCs?


May 30, 2012, 11:50 

#36 
Senior Member

Velocity inlet with 40 m/s (X direction), Intensity and Viscosity Ratio (1% and 10 %), Pressure outlet is at 0 gauge pressure obviously and also Intensity and Viscosity ratio (5 % and 10 %), ahmed body and the ground are stationary walls and symmetry, side and top are all symmetry (which is the same as a noshear stress wall).


May 30, 2012, 12:11 

#37 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Why 1% turbulence intensity? I set it to 2.5, but i wil try with your settings. Now i velocity inlet with 40m/s and ambient pressure, pressure outlet at the same ambient pressure ( with operating conditions set to 0, so it should be the same). Why do you use symmetry and not noslip wall? It has a physical meaning or just for simplicity?


May 30, 2012, 12:15 

#39 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 
Sorry I set turbulence intensity at 0.25% which is the upper limit of the wind tunnel


May 30, 2012, 12:16 

#40 
New Member
alessandro
Join Date: Oct 2010
Posts: 28
Rep Power: 7 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
No layers in a small gap  bobburnquist  OpenFOAM Native Meshers: snappyHexMesh and Others  6  August 26, 2015 09:38 
Polyhedral Mesh Quality in StarCCM+  niazaliahmed  STARCCM+  3  March 8, 2012 14:51 
[ICEM] Tetra mesh quality before and after prism layer  Chander  ANSYS Meshing & Geometry  0  December 25, 2011 23:04 
fluent add additional zones for the mesh file  SSL  FLUENT  2  January 26, 2008 12:55 
Icemcfd 11: Loss of mesh from surface mesh option?  Joe  CFX  2  March 26, 2007 18:10 