What is the 'ideal' manner for meshing near a blade? To be more specific, should the nodal density require a number of nodes within the estimated boundary layer, and if so, could it be approximated with flat plate given no experimental data?

Given a nodal budget, the first grid may be coarse and then adjusted based on bl, etc; however, for in a turbomachinery problem, we require a high number of nodes to capture torque (viscous,etc) while the pressure 'apparently' is not as grid dependent.

I realize that this may be somewhat of a general question, but I appreciate any and all input. Are there any good books on the use of grid?

(1). Study and plot the velocity profile in a turbulent boundary layer. See book by Schlichting's "Boundary Layer Theory" (every library should have it). (2). Run a series of 2-D flow through turbine cascade, with various mesh stretching near the wall at different stations along the boundary layer. (3). Since the boundary layer thickness varies along the blade, the mesh and mesh stretching must change accordingly. You can run your numerical experiment to check the results. (4). If you don't have enough mesh points, try the high Reynolds number option with wall function treatment. (5). If you still do not have enough mesh points, the results probably are not going to be accurate. It is still all right, because not everybody cares about the accuracy of the result.

Hi John,

what do you mean "nobody cares about the accuracy of the result"? I do know, from my experience, that very few people understand the issues of accuracy especially with respect to gridding BUT I think a lot of people do care about the accuracy as they are actually building, optimizing and running the equipment which is being simulated.

I think the problem is finding the right ballance of compromise between pure academic accuracy and practical time/energy/effort constraints. We like to think that computers are the majic answer to our problems but the more experienced people know that this is not true!

Regards.......................................Duan e

Is it really good to stretch the boundary layer mesh in the normal direction when you come further downstream in order to match the boundary layer growth? It might seem like a good idea, but I'm not convinced that is the case.

For most numerical schemes it is very benefical if the cell-centers and the face-centers of the cells in the boundary layers are on the same distance from the wall - there are very strong gradients in the direction normal to the wall and very small gradinets in the direction parallell to the wall. If you stretch your grid in the normal direction when you go downstream you will not have cell-centers exactly aligned with face-centers.

Any opinions on this matter?

(1). I will try to make it easier to understand. (2). Since the boundary layer thickness will vary from the leading edge to the trailing edge, one should have enough mesh points inside the boundary layer at any station. Otherwise, you are not going to see the boundary layer accurately. (3). This is assuming that you are using low Reynolds number turbulence models. In this case, the first mesh point away from the wall must be located within the viscous sublayer, or ideally within Y+ less than one. (4). When using the wall function, the constraint is somewhat different, because in this case, the first point away from the wall must be in the fully-turbulent region.(say Y+ larger than 50) (5). The mesh must be adjusted based on the computed results to satisfy the above mentioned requirements.

(1). I said,"...not everybody cares about the accuracy of the results." (2). You changed it into, "nobody cares about the accuracy of the result." (3). I can only say that, "me no English ! " Sorry, I don't understand. (4). As to the level of engineering solution accuracy, a solution within 5% of the true solution would be considered acceptable. I think, in most cases, we are not there yet. (pressure distributions, maybe.)

The wall function case is special - then you don't have any choice but to stretch your grid in order to keep y+ of the first cell reasonably constant.

In the low-Re case you have a choice though, and as I argued in my previous post, there are numerical advantages with not stretching the grid. Stretching your grid might save you a few cells but you might loose more in the end because you have to use a better resolution in order to obtain the same accuracy.

(1). Let me say it the other way around. Let's assume that, near the trailing edge on the suction side surface, we have 30 points inside the boundary layer. Using the low Reynolds number model, we should try to set the first point away from the wall to within Y+ =1. (2). Then on the forward portion of the suction surface, the boundary layer will be thinner there. Instead of stretching the mesh, now, we can compress the mesh (near the trailing) and fit it inside the thinner boundary layer. This will be consistent with the boundary layer behavior. (3). In the thinner boundary layer, one still have to check the first point Y+ value to make sure that it is within Y+ =1 constraint. (4). In this case, the distance from the wall to the first point will change along the surface. Whether this will affect the numerical accuracy or not depends on the mesh type used near the wall, and the treatment of the boundary conditions there.

Very interesting.

>there are very strong gradients in the

>direction normal to the wall and very small gradinets ...

Kghm, Jonas, but my grid steps are not the same in normal and tangential direction. I try to choose the step ratio in such a way that while du/dx and du/dy are very different, du/di and du/dj are of the same order. And this is du/di and du/dj what really counts.

Sergei