CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Simple question? On mesh aspect ratio on boundaries (http://www.cfd-online.com/Forums/main/73606-simple-question-mesh-aspect-ratio-boundaries.html)

TfG March 12, 2010 05:03

Simple question? On mesh aspect ratio on boundaries
 
Hi all,

I keep reading and hearing about problems that mesh elements with high aspect ratio can give. However, I keep seeing that boundary mesh next to the wall have really huge aspect ratios. Canīt that give convergence problems? Or is it that somehow in the boundaries where boundary layers are expected somehow it helps more than worsen the problem?

Thanks

agd March 12, 2010 09:54

Generally speaking a poor aspect ratio can cause convergence problems. What you see when you look at a lot of grids is the tradeoff of practical run-times versus aspect ratio - i.e. we accept worse aspect ratios than we might like in order to keep the number of grid points down to a realistic number. We do have one benefit in boundary layers in that the gradients in the streamwise direction are smaller than the transverse gradients, so the large aspect ratio is not as much of a problem as it could be (unless you have to deal with separated flow).

jchawner March 13, 2010 17:29

TfG: I agree with what agd wrote and add these minor issues. For structured quad/hex grids high aspect ratios in the boundary layer cells are the norm and depending on the solver you can handle ARs of 10,000 or more. However, you still have to keep in mind the effect that those long cells are going to have on accurate representation of the true shape of a curved boundary.

Also, the issue of AR gets more complicated when you consider tri/tet unstructured meshes. A high aspect ratio triangle can have really poor included angles and that will destroy mesh quality. Put those in the boundary layer where you want to resolve large gradients normal to the wall or use a wall function and all bets are off in terms of accuracy.

Hope this helps.

TfG March 14, 2010 18:03

thanks for the info. really helpful

wxmoore January 8, 2013 11:38

My understanding is that high aspect ratio cells are less problematic if they are located within the boundary layer near the wall where the flow velocity normal to wall is generally low. In addition, in order to achieve the recommended y plus of +1 or less for enhanced wall treatment or k-omega SST turbulence models then it is recommended to use at least 10 inflation layers and preferably 15 or higher to provide high resolution inn the viscous sub layer and smooth transition to the turbulent region. For example the model that I am cuurently using has 15 inflation layers for tet prism layer mesh with a max cell skewness of 0.89 and a max aspect ratio of 100 near the walls. The minimum orthogonality is 0.15.

This mesh appears to give much better convergence than model based on using only 5 to 7 inflation layers, with higher y plus values.

Anna Tian January 30, 2014 06:19

Quote:

Originally Posted by agd (Post 249711)
Generally speaking a poor aspect ratio can cause convergence problems. What you see when you look at a lot of grids is the tradeoff of practical run-times versus aspect ratio - i.e. we accept worse aspect ratios than we might like in order to keep the number of grid points down to a realistic number. We do have one benefit in boundary layers in that the gradients in the streamwise direction are smaller than the transverse gradients, so the large aspect ratio is not as much of a problem as it could be (unless you have to deal with separated flow).

What if we have separated flow? I'm currently having aspect ratio in the boundary layer of about 30000 for the wing simulation. It doesn't bring convergence problem when there's no BL separation. According to what you say, I won't doubt much about the inaccuracy of the modeling introduced by the current high aspect ratio. This is also verified by my tests. But I'm wondering, if we have separated flow, what problem would the high aspect ratio grids introduce?

agd January 30, 2014 21:45

When the flow separates it means that the gradients along the surface can be significant. A large cell aspect ratio simply means you have to be concerned that you are lacking tangential resolution to capture those gradients - so you may get inaccurate results for things like the location of a separation point. It's the same reason why we typically cluster grid points near leading and trailing edges. Unfortunately, separation location is not always so easily predictable, so this is just one more thing you have to consider and possibly justify/correct after making an initial run.

Anna Tian January 31, 2014 06:49

Quote:

Originally Posted by agd (Post 472679)
When the flow separates it means that the gradients along the surface can be significant. A large cell aspect ratio simply means you have to be concerned that you are lacking tangential resolution to capture those gradients - so you may get inaccurate results for things like the location of a separation point. It's the same reason why we typically cluster grid points near leading and trailing edges. Unfortunately, separation location is not always so easily predictable, so this is just one more thing you have to consider and possibly justify/correct after making an initial run.

What's the reason that we typically cluster grid points near leading and trailing edge? Because the gradients at leading and trailing edge are larger than the other parts?

Will very large aspect ratio cause any additional problem besides the considerations from the view of discretization error? You know, typically software tutorials on grids quality requirements suggest that the aspect ratio need to be smaller than 5000.

agd January 31, 2014 09:45

Clustering is used at leading and trailing edges because at attachment and separation points we want to capture the gradients that show up. The question arises when we don't have separation or attachment at a known location. Then the question is where do we need to have decent tangential resolution? Another issue that presents itself in highly stretched cells, especially in FV schemes, is the reconstruction of the overall gradient. It has been shown that weighted least squares is better than Green-Gauss most of the time - however one of the regions where Green-Gauss seems to be better is in viscous regions where the grid cells are highly anisotropic. So depending on how your solver is reconstructing the gradient there may be some additional issues with highly stretched cells.

Anna Tian February 1, 2014 07:08

Quote:

Originally Posted by agd (Post 472800)
Clustering is used at leading and trailing edges because at attachment and separation points we want to capture the gradients that show up. The question arises when we don't have separation or attachment at a known location. Then the question is where do we need to have decent tangential resolution? Another issue that presents itself in highly stretched cells, especially in FV schemes, is the reconstruction of the overall gradient. It has been shown that weighted least squares is better than Green-Gauss most of the time - however one of the regions where Green-Gauss seems to be better is in viscous regions where the grid cells are highly anisotropic. So depending on how your solver is reconstructing the gradient there may be some additional issues with highly stretched cells.

Is RANS model able to predict Cl accurately when the wing is already stalled? Could higher tangential resolution help on that? Or higher tangential resolution could help on accuracy of the stall angle of attack prediction?

agd February 1, 2014 22:50

RANS models can be used to compute the lift coefficient for stalled airfoils. But as I have stated, the location of the separation point will be affected by the tangential resolution of the grid. Inaccuracies in the location of the separation point can have an impact on the accuracy of the lift calculation. How much of an impact is something that should be determined using your flow solver.

Anna Tian February 2, 2014 06:59

Quote:

Originally Posted by agd (Post 472931)
RANS models can be used to compute the lift coefficient for stalled airfoils. But as I have stated, the location of the separation point will be affected by the tangential resolution of the grid. Inaccuracies in the location of the separation point can have an impact on the accuracy of the lift calculation. How much of an impact is something that should be determined using your flow solver.

In my tests of the 3D wing CFD, the grids independence is already verified. Finer grids do not change Cl and Cd anymore. And in the comparison with experiment, I found that the larger angle of attack is (larger area of BL separation), the larger discrepancy to experimental data is. Shall we say that CFD is worse at higher angle of attack prediction than at low angle of attack because of the limit of the RANS model? Is this a common experience and conclusion?

agd February 2, 2014 15:46

Lift at the onset of stall can be computed using RANS models, but the typical calculation today will generally use a detached eddy version of the basic turbulence models. These will give better results, but the question of accounting for the correct separation/reattachment points still exists. A coarse grid (or a fine grid that is too coarse in the regions of separation and reattachment) can play a role in the accuracy of the lift and drag as well. How much of a role is generally problem dependent, and depends also on what you are trying to get out of your simulation.

Anna Tian February 3, 2014 11:48

Quote:

Originally Posted by agd (Post 473017)
Lift at the onset of stall can be computed using RANS models, but the typical calculation today will generally use a detached eddy version of the basic turbulence models. These will give better results, but the question of accounting for the correct separation/reattachment points still exists. A coarse grid (or a fine grid that is too coarse in the regions of separation and reattachment) can play a role in the accuracy of the lift and drag as well. How much of a role is generally problem dependent, and depends also on what you are trying to get out of your simulation.

What do you mean by 'detached eddy version of the basic turbulence models'?

agd February 3, 2014 16:46

See

http://www.cfd-online.com/Wiki/Detac...tion_%28DES%29

for details.

Anna Tian February 5, 2014 04:42

Quote:

Originally Posted by agd (Post 473017)
Lift at the onset of stall can be computed using RANS models, but the typical calculation today will generally use a detached eddy version of the basic turbulence models. These will give better results, but the question of accounting for the correct separation/reattachment points still exists. A coarse grid (or a fine grid that is too coarse in the regions of separation and reattachment) can play a role in the accuracy of the lift and drag as well. How much of a role is generally problem dependent, and depends also on what you are trying to get out of your simulation.

Have you even ran the simulation for stall flow? Will transient simulations be always necessary for the convergence if fine enough mesh is used?

agd February 5, 2014 10:47

I have run stall simulations for the NACA0012, NACA0015, and NACA63-018, among other profile shapes. I always run my simulations in time-accurate fashion, so I cannot answer your last question.

Anna Tian February 5, 2014 10:54

Quote:

Originally Posted by agd (Post 473566)
I have run stall simulations for the NACA0012, NACA0015, and NACA63-018, among other profile shapes. I always run my simulations in time-accurate fashion, so I cannot answer your last question.

You mean the simulations you ran on that are all transient? Have you tried 3D simulation on that?

agd February 5, 2014 15:18

I don't run simulations in steady state mode. I always use a time-accurate solver for my simulations, whether 2D or 3D.

Anna Tian February 5, 2014 16:01

Quote:

Originally Posted by agd (Post 473613)
I don't run simulations in steady state mode. I always use a time-accurate solver for my simulations, whether 2D or 3D.

I found that the transient and steady-state simulations will give exactly the same results if both of them converge for 3D case. Probably transient simulation is just for a convergence issue.


All times are GMT -4. The time now is 23:22.