Hi, I'm still Gabriel. I would like to know if anyone can tell me something about the aspect ratio (of a cell) to be used in a finite volume simulation. Is there any particular rule? How the solution change?

Thank you.

There are many reasons for a particular aspect ratio.

A physical reason is: the structure of the flow. If you know that the structure of the flow will not be homogeneous then you might want to consider a given aspect ratio. For example if you have a boundary layer, with a strong shear in it, then in the direction normal to this boundary you want to have a higher resolution (and smaller grid spacing) to resolve the boundary layer. While in the dimension parallel to the boundary you can have a larger grid spacing. If you know that you have waves in the flow, then you want to make sure to resolve them in each direction with a least a few grid point in each dimension (say at least 6 points per wave length). Since the waves might be propagating in each dimesion with a different speed (because of the angle of propagation), then in each dimension (direction) you need to have the appropriate number of grid points.

These are physical reasons, there are other reasons which might be due to the specific numerical schmeme you are using and so on.

Any other suggestion?

Patrick

Another question. Is there any empirical or theoretical rule to calculate the best aspect ratio, for example in a pipe, with the longitudinal direction much longer than the others two,in which a longitudinal flow created by internal jet-fans takes place? Thank you very much, Gabriel

I don't know of any rule or theoretical law in general. Again, one needs to know things such as

are the boundary effects important?

is the flow laminar or turbulent?

is the turbulence homogeneous?

are there streamwise vortices in the flow?

and so on..

In short it would be wise to have some basic experiments that tell you qualitatively about the processes in the flow, and the simulations are to evaluate these processes quantitatively.

For example if the flow is laminar and a boundary layer develops at the (inner) surface of the pipe. Then I would guess that the cells can be elongated in the direction of the flowing fluid in the pipe, their width decreasing in the boundary layer (making them even more elongated).

Or, if the flow is fully turbulent, I would guess that you need the same resolution in all dimension (cubic cells), with an increasing number of points in the boundary layer if it is of small size only (making the cells elongated next to the boundary only).

etc..

PG

In a finite element analysis (structural, for example) the rule of thumb is to try to have an aspect ratio of as close to 1:1 as possible. Generally FEA codes will not have problems with aspect ratios of 5 or 10:1.

CFD is a completely different beast. Because of the nature of the simulation, it is not unusual to have aspect ratios of more than 1000:1. It is hard to define a rule of thumb for acceptable aspect ratio that doesn't require the analysist to have some "feel" for the solution. The most concise advice I can give would be to echo Patrick's advice that the grid has to be fine enough to capture the gradients in the physical flow.

In most cases, such as flow in a pipe, there is one direction that will have larger flow gradients than the others, in this case the radial direction. The grid in that direction will require refinement (or clustering) in the high gradient regions near the wall. The required grid spacing at the wall is going to depend on the turbulence model that is being used and the resolution desired. Required y+ values of 5 are not uncommon.

In the streamwise direction, the grid should contain enough resolution to capture changes in geometry. If the grid is in a 90 degree pipe elbow, you might use 30 nodes in the streamwise direction (one node every 3 degrees). That grid would be fine enough to capture the curvature of the geometry, and the flow gradients that causes.

You'll probably find that your own experiences will provide the best guidance for determining if a mesh is sufficient.

Gabriel,

Aspect ration of a computational cell cell can be defined as a ratio of minimum height to maximum base. This definition may however be questionalble, but I base my reply on this definition.

Why does one need high aspect ration cells (also called stretched cells). Well it saves the grid smaller (less number of cells). How can one use streched cells. Because certain regions in the flow may be known to have stronger gradients in one direction than others. Such is the case for boundary layers, shear layers, shocks ... So when initial mesh generation is done this apriori information about the flow is utilized to generate cells with that would resolve the flow gradients in each flow direction (ideally) with equal accuracy. Since this ideal is difficult to achieve without knowing a solution, a qualified guess is often used (for example mesh clustering normal to a no-slip surface is often determined by y+ criteria, which is the normal distance from the surface normalized by a viscous length scale).

Once an initial solution is achieved on an initial mesh (which was built with some prior knowledge of the flow which is typically available), the mesh can be regenerated, or modified (adapted by local refinement and corsening based on flow gradients). This new mesh, ideally would resolve gradients in all spatial directions equally well. This process would also, ideally, result in a mesh that has the same level of discretization error through out the flow field.

Most of the "automatic" mesh generation tools available today do not produce streched cells (I would love to be proven wrong on this one). Similarly, i do not know of any commonly available mesh adaption tool that produce anisotropic refinement and grid adjustment at the same time (again, tell me otherwise if you know of some tools).

Let me throw in another thing. Streched cells may be good for only a few of commonly used cell types. for example, for a 2D mesh, stretched rectangles may be good, but streched triangles are not since this results in very skewed cells and solution accuracy is compromised. For 3D, prisms (one directional streching), or stretched cubes (for two-directional streching)would be good choices, while streched tetrahedra are bad because of skewness considerations.

In summary, if the flow field is spatially uniform, a mesh with isotropic cells would be the best choice. If the flow has anisotropicity in some regions, then a proper use of strteched cells would save on numbner of grids. Of course isotropic cells can also work, but they would be unnecessary and can result in a mesh even ten times larger (or even more. see Alton's message 50:1 cells, so if one insists on using 1:1 one can easily end up with 50 times the grid with no added accuracy).

This was my 2 cents worth. Why do I have so much free time on Christmas eve! Merry Christmas and happy holidays to all of you.

Faraz,

I know of one mesh generation tool that might be considered "automatic" that does generate stretched cell meshes, and seems to work well. It is VIScart from CFD Research Corp. It works on imported surface gemoetry from a CAD package. You (the user) define a number of parameters that govern what the mesh will look like including the desired perpendicular spacing at the wall and in the "free stream". The code then applies a fairly standard looking mesh in the boundary layer near the walls and then used a cartesian mesh in the rest of the domain.

It's fairly fast, and I think of it as mostly automatic. If it could read my mind and save the typing, then it would REALLY be amazing.

I had a look at it. Some cells in the transition from layers to the cartesian region look rather bad. Secondly the volume ratio of adjacent cells is, as far as I can tell, easily as high as 8:1! I wonder how it is going to affect the solution accuracy.

But thanks for correcting me.