CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Mesh Quality (http://www.cfd-online.com/Forums/ansys-meshing/102540-mesh-quality.html)

alenglaro May 27, 2012 17:33

Mesh Quality
 
1 Attachment(s)
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

Far May 28, 2012 00:31

Can you attach the .tin and .blk files?

alenglaro May 28, 2012 05:36

.tin and .blk files
 
1 Attachment(s)
Thank you very much!

Far May 28, 2012 07:02

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.

alenglaro May 28, 2012 07:47

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

Far May 28, 2012 08:51

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?

Far May 28, 2012 09:02

Quote:

Originally Posted by alenglaro (Post 363425)
where do you see that
Thanks

In fluent, I check it

alenglaro May 28, 2012 09:04

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

Far May 29, 2012 01:28

Quote:

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).
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..

Quote:

The strange thing is that in icem those elements are marked as high quality
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.

Far May 29, 2012 02:06

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.

scipy May 29, 2012 03:10

Quote:

Originally Posted by Far (Post 363504)
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?

Far May 29, 2012 04:35

Some thoughts
 
Quote:

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


Quote:

I've managed to get 1 % agreement with experimental results with a hybrid prism/tetra mesh for the same domain
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.

alenglaro May 29, 2012 04:57

Quote:

Originally Posted by Far (Post 363497)
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.

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

alenglaro May 29, 2012 05:05

Quote:

Originally Posted by scipy (Post 363510)
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).

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)

Far May 29, 2012 12:41

blocking
 
1 Attachment(s)
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).

Far May 29, 2012 12:51

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

alenglaro May 29, 2012 13:20

1 Attachment(s)
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?

Far May 29, 2012 14:08

turn off the solid and VORFN


Quote:

.atr or .fpb
these files are not important, just press cancel.

alenglaro May 29, 2012 14:29

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

Far May 29, 2012 14:31

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


All times are GMT -4. The time now is 05:26.