[Far]

I still believe that you should extend the domain. But first try with this domain and then compare results with extended one.

[Far]

I had problems in meshing same geomtry in ICEM, four months ago.
http://www.cfd-online.com/Forums/ans...d-vehicle.html

I was making one silly and small mistake in that blocking. Could some point-out , what was it?

[alenglaro]

Did you have difficulties on convergence? I see that with k-e 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

[Far]

which mesh you are using. Use far3

[alenglaro]

I'm actually using far3. What do you suggest?

[Far]

we have good convergence and drag is 0.275. (scipy is running it)

[alenglaro]

What settings and turbulence model?

[Far]

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.

[alenglaro]

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

[Far]

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.

[scipy]

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 30-50 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 (8.2-3 sec per iteration).

[alenglaro]

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

[scipy]

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..

[Far]

Regular steady state and then Coupled instead of SIMPLE, Courant number is there under solution controls (i used 50

He is talking about the pressure based coupled solver. fourth option whereas SIMPLE being the first option (SIMPLEC, PISO and Couple). This Courant is somehow different than the Courant no. of density based coupled solver.

[alenglaro]

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?

[scipy]

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 no-shear stress wall).

[alenglaro]

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 no-slip wall? It has a physical meaning or just for simplicity?

[Far]

@alenglaro: Can we shift this discussion on Fluent forum?

[alenglaro]

Sorry I set turbulence intensity at 0.25% which is the upper limit of the wind tunnel

[alenglaro]

Originally Posted by Far

@alenglaro: Can we shift this discussion on Fluent forum?

Yes you are right I'm going to create a new topic