Mesh Quality
 

Hello,
I'm trying to mesh an ahmed body in ICEM. As you can see in the picture I achieved a fairly satisfactory result. Premesh quality is above 0.5, as well as orthogonal quality once i converted premesh into unstructured mesh. Determinant is above 0.75, min angle between 26 and 100 degrees. Tgrid skew (if it's meaningful for hexa elements) is less than 0.65. Apparently should be ok but when I import the mesh into fluent i get a warning about wall distance (probably due to high aspect ratio elements in the boundary layer) and the orthogonal quality (in fluent) is lower than 0.1.
Only if I increase first boundary layer thickness from 0.01 (that I need for the mesh) to 0.1 or higher quality rises above 0.5.
What's wrong and what can i do? Why ICEM tells me that's a good mesh when fluent thinks it's not?
Thank you very much

Can you attach the .tin and .blk files?

.tin and .blk files
 

Thank you very much!

the minimum orthogonal quality is 0.08 and required is 0.05 (or 0.01 I am not sure). The blocking is very good, however edge mesh parameters setting is not good. Try to improve edge bunching and you will even get higher quality.

where do you see that? in orthogonal quality icems shows me a minimum quality of 0.5. How can I improve edge parameters? Any advice?
Thanks

I meant that the transition of meshing between two blocks should be minimum. Do not copy the meshing, on the bod,y to farfield, in this way you will get cells with very high aspect ratio and low quality. These cells also disturb the convergence.

did you check the mesh in Fluent? are you still getting the warning about the mesh quality?

In fluent, I check it

Yes I checked in fluent the mesh i attached here and asks me to repair wall distance. quality about 0.09, very low, and the simulations goes overflow (even in dp). Maximum aspect ratio over 30k (far from the body). I plotted contours of mesh quality in fluent and the worst elements are in the frontal-lateral surface of the ahmed body (the curved surface). The strange thing is that in icem those elements are marked as high quality

Wall distance is the another measure of aspect ratio. It is required by SA and two equation omega based models. You should avoid the high aspect ratio at the far field. Higher aspect ratios are allowed (upto 1000 for dp), but I have also tested the aspect ratios up to 8000-10000 for NASA rotor 37 and results were still comparable to experiments with 2-3% error.

So rule of thumb is that you can go for higher aspect ratios (1000-10000 with dp) in boundary layer but you must avoid them in far field.

Minimum orthogonal quality required is 0.01 and if you are getting problem then you should check settings in Fluent, such as under-relaxation parameters, mesh scaling, mesh units, boundary condition etc..

What is the quality (numeric value) of these elements in ICEM?


I am also attaching another blocking today with some minor changes. It has somehow higher quality, although with simpler blocking.

PS: For simulation related problems, post a thread on Fluent (or CFX )forum and we can discuss this there in detail.

Oh, I check the domain extents and they are too close to the body. Body length is approx. 1000 units and downstream is 5000 units (5 lengths) and upstream boundary is 2000 units (2 lengths). And the flow is low subsonic. For this you need at least 10-15 lengths upstream and 20-30 lengths downstream. Similarly 10-15 lengths in Y and Z direction.

I think he's actually trying to replicate the results of the LSTM wind tunnel testing on the Ahmed body done by Lienhart and that wind tunnel is 1.4 m high, 1.87 m wide (so half of that since symmetry is used), the downstream length is 5L (5*1044) and upstream of 1.3L (he chose 2L).

I've managed to get 1 % agreement with experimental results with a hybrid prism/tetra mesh for the same domain, so I wonder, is the necessity for a larger domain purely because of the hexa elements or? Since I thought they were higher quality elements and as such should experience even less problems than tetras?

In any case, I know for a fact that people from the car industry recommend upstream of about 7-10L max (or at least 100 cells in the direction of the flow before the stagnation point) and downstream of 12-15L, so, why the need for 30L?

Some thoughts
 

Very good information and thanks for sharing. I didn't know this before.


Once I talked to Dr Florain Menter (Or Dr Knopp from DLR http://num.math.uni-goettingen.de/knopp/)on same aspect that the my results with this model and this mesh are closer to experiments and with this other model and mesh (better model, mesh and Y+) are away from experiments. He replied that "in CFD it is important you should follow the systemic approach rather than comparing to experiments (although it is also important, but this should be done when you are fine tuning physical model). For example we all know that K-epsilon model is not good at predicting the stall as compared to SST model, but if you are getting close results then this is due to fortunate cancellation of errors rather than accuracy of physical model.

The check would be the sensitively analysis. Take three domains with 2 lengths downstream, 15 lengths downstream and 25 lengths downstream with fixed upstream 15 lengths.

Using Orthogonality quality criterion those elements are above 0.8 but i think that's not the same criterion used by Fluent. What criterion should I check? In icem worst elements are on the lateral corners of the body, but this make sense
Could you please attach your mesh please? Thank you

Yes I'm trying to replicate that experiment. For now I'm only doing a mesh convergence study, with a basic k-epsilon model, surprisingly obtaining a good prediction of cd (less than 2% error, despite a first boundary thickness of 0.1mm and an y+ between 3 and 80)

blocking
 

I am attaching three blocking schemes, almost similar in general layout, but different in edge mesh parameters, edge settings etc. This has also huge impact on the quality. With case 3, I am getting orthogonal quality of 0.2 with very fine mesh in boundary layer (I guess Y+ is order ~1, please confirm it and let me know).

Pics
 

http://img713.imageshack.us/img713/8881/82164898.png
http://img26.imageshack.us/img26/1229/23902882.png
http://img502.imageshack.us/img502/3051/90000019.png
http://img443.imageshack.us/img443/2505/93024194.png
http://img805.imageshack.us/img805/6830/63482277.png
http://img31.imageshack.us/img31/4600/98380759.png

Thank you for your help, but when I load your files .prj icem tells me that file .atr or .fpb is missing and the premesh looks distorted as you can see in the picture. What's wrong?

turn off the solid and VORFN


these files are not important, just press cancel.

Ok now it works. I'm going to launch simulation. Why you use material point? What is its utility?

material is used to define the fluid region/solid region in 3d

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

funny
 

I had problems in meshing same geomtry in ICEM, four months ago. :o
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?

:) 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

which mesh you are using. Use far3

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

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

What settings and turbulence model?

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.

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 :)

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.

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:

http://i.imgur.com/Gfhqe.png

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:

http://i.imgur.com/YFKvX.png

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:

http://i.imgur.com/lTQvr.png

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).

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

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..

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.

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?

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).

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?

Solver forum
 

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

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

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