Hi,

I found that for different papers investigating similar flow phenomenons, their grid resolution differs by quite a bit.

For e.g., a paper by Tuncer investigating moving airfoil at Re=1x10^4 uses a c-grid 181x81 size for computation, with a compressible NS solver.

Another paper by Young, with similar solver and test parameters, uses a c-grid 1081x121, with the 1st normal grid pts at 9.2x10^-5 from surface. The only difference is that Re is now 2x10^4.

Although the Re is twice of the above, the grid resolution and near wall distance are much higher. So is the latter using too high a resolution? Or is the former's resolution too low.

Is there a standard for different Re? Or as long as higher resolution does not cause a change in the results, the lowest one is used.

Thanks.

It depends from the accuracy you require as well. I believe that a study of the grid dependence is necessary before you can accurately solve any problem. In any case, if your solver is not using any wall functions, you need to go as down as y+ of the order of 1 to solve the boundary layer correctly. You could reduce the computational cost by using wall functions (your y+ will be of the order of 30 in this case). It is likelt that the two papers you cited differ in this. I don't think the Reynolds number difference is an issue (fairly similar ...)

Judging by the cell size off the wall (assuming the number you're giving is non-dimensional by chord), Young is most certainly trying to resolve the boundary layer. You may check for reference to wall-functions in Tuncer's paper, but also keep in mind that many older papers cite astonishingly low cell counts simply because that's all they could afford to run with their computing power at the time. That doesn't necessarily mean it's adequate. Such questions are all the more reason to call for a grid resolution study which would reveal if the resolution is insufficient or excessive. Some (if not all) CFD journals would reject a paper if results are shown only on a single grid.

Mani:

What you do when you have a mesh size of 4-5 million cells and you cant reduce that because of the geometry. I am talking about hexahedral mesh not tetrahedral. In this case what do you do about grid study?

Munni

I reckon it depends on what you are trying to achieve. If absolute accuracy is what you are after, you have no choice, you just have to go through the mesh sensitivity study. However, if you are using the CFD work in design, you are most likely interested in differences between different configurations or conditions. The important thing then is to keep the mesh very consistent across all your runs. Purists may argue that you still need to do the mesh independence study anyway, but reality is that the project will then most likely be over long before your CFD results become available! For DESIGN purposes (where you need to investigate the relative effects of certain parameters), one can often contribute most to the process with CFD runs that are nowhere near mesh-independent. You can only get away with this if there are more detailed further checks (such as wind tunnel tests) further down the line.

Hi Tiz,

By using the viscous grid spacing calculator, entering a Re of 2x10^4, y+=1, in non-dimensional terms results in a spacing of ~7.7e-4 units.

However, the paper by Young has the 1st normal grid pts at 9.2x10^-5 units from surface. even if he is trying to solve the boundary layer, isn't that an overkill?

Or is this because it is an unsteady moving airfoil problem? Hence the y+ value must be much higher.

Mmmm .... firt of all, the lower y is the lower is y+ (there is some inconsistency in your formulation).

I have dome some sensitivity studies in the past ... (the problem is slightly different) and I get grid independence for a value of y+ of the order of 1. By using a wall function, I can sensibly reduce the computational requirement and I get basically the same results with a y+ of the order of 30. However, with separated region the use of a wall function ruins the computational accuracy and I have to go back to the lower y+ to get the right solution.

And by the way, remember that the boundary layer grows on the wing, so that the initial Reynolds number is much lower than the reported one (the Re that drives BL thickness). Young is probably trying to achieve a y+ of the order of 1 across the whole wing...

Hope this help

Tiz

Have a look at the PhD Dissertation of young.Its available electronically.It discusses the questions that you posed.

Munni,

what geometry is that, that does not allow you to reduce the grid count below 4 Millions? I can understand how locally the resolution is set by small features, but globally in the whole domain?? If that's the case, your grid resolution must already be at a bare minimum (with 5M!). I am curious what type of geometry that is, but I actually wasn't referring to your grid. I was referring to the published papers Ben mentioned. Those are very simple grids that can easily be subjected to a grid resolution study, and I am guessing that this was actually done.

>By using the viscous grid spacing calculator...

I can see how an order of magnitude difference makes you wonder (I don't see the inconsistency you are referring to, tiz).

Nevertheless, remember that those "grid spacing calculators" only give you an estimate of appropriate cell size based on empirical data, typically for a flat plate. The "overkill" may either be intentional to be on the safe side, or it may be indeed the result of a grid resolution study. You're also right that the unsteadiness may increase the requirements on resolution considerably, especially if you have separation. I guess you'll have to do what Harish suggests and check out the thesis.

This is the inconsistency

"Hence the y+ value must be much higher."

He clearly meant lower ...

I forgot to post the link to the thesis.Here it is

http://www.library.unsw.edu.au/~thes...143413/public/

I remember seeing an AIAA journal paper of young and Lai.If I'm not wrong,the work of young is an extension or improvement of the work of tucker.

Thank you all for the suggestions.

I have read Young PhD thesis. It seems that the reason for using such fine grid resolution is to resolve the wake structures.

By the way, both of them use the reynolds-averaged NS eqns. Accuracy aside, does using this simplified form has an influence on the grid resolution?

That is, at the same Reynold no. and solving the same problem, will there be a difference in the grid resolution if the normal and simplified eqns are used?

If so, which one will require a finer grid? Is it the normal NS eqns?

I think the point is exactly the opposite. Using RANS allows you to use such a coarse grid because you are not actually solving the turbulence structure of the flow but using a model for it (regardless of which ... algebraic - k-espilon, k-omega or Reynolds stresses ...).

I you were to resolve the NS equation directly (DNS) you would have to ensure you are able to capture all the turbulent structure (from the big eddies to the small eddies were dissipation occurs). It is quite a complicate subject and I am not going into details here but you'd need millions of grid points even for a very simple problem (and of course you couldn't do a 2d simulation as turbulence is inherently tri-dimensional ...)

Tiz

>If so, which one will require a finer grid? Is it the normal NS eqns?

Yes, exactly. It's the "normal" NS equations that require high resolution, not the "simplified" Reynolds-averaged equations. The difference in required resolution is extreme and prohibitive, so don't even think about using the direct approach to turbulence.

of course...