Does anybody has experince with CFX 4.2 CFD program package? I am trying to learn using it, so any help in it would be appreciated.

Zoltan,

For pre-processing (that is, generating the grid to define your model), look at page 3 of the Examples manual, it has a number of reasonably well documented examples to get you started. On-line help in CFX-Build is quite good, press F1 to get help on whatever the mouse pointer is on.

For the command file and fortran routines (which define the fluid, solver and other parameters required to define the model) the best advice I can give is to choose an example from the example and reference example list which is closest to what you want to model, an go from there. The list is on page 289 of the Examples manual.

Hope that helps, Glenn

Dear Glenn!

Thank you for your help. I worked through the examples on pre-processing, but i found only few things about the grid generation. Building the geometry acording the examples is straight forward, but what i missed are some rule of thumb. For example, the same geometry can be created on several ways, some of them is acceptable for gridgeneration some of them are not. how can i decide it. Other thing is witch method should i used for my geometry: isomesh or paver , and so on. I know this is because i am a dummy in CFD yet, but i want to learn it. So that why, i need some rule of thumb i can follow on my learning path. Thank you again Best regards

Zoltan Turzo

Zoltan,

Paver vs Isomesh: The simple answer is Isomesh is a structured surface mesh generator. Paver is unstructured. CFX 4.2 uses structured mesh, so you should use Isomesh. (I understand that it is possible to use paver to mesh a 2 dimensional unstructured shape, and then extrude that mesh in the 3rd dimension. I've tried this and never got it to work. Any suggestions anybody?)

If you are asking what is structured vs unstructured meshes, a quick answer is: A node in a structured grid can be identified by 3 coordinates, i,j,k. The node's neighbours will be i+1, i-1, j+1, j-1 etc. It need not necessarily be rectangular. A node in an unstructured grid is identified by 1 parameter, just a node number. The node's neighbours are determined by a seperate "connectivity array", which defines how the nodes join together - node 312 to node 234, 23, 534 etc.

As for "rules of thumb" in mesh generation, the things you have to look out for are the quality of your mesh. This is THE major factor in determining the quality of your solution, regardless of whether you are using CFX, Fluent, your own code or what ever - even structured or unstructured.

Things to try to optimise include:

Cell angles - for a structured mesh, try to the angles of the cells as close to 90° as possible. (60° if your elements are triangles)

Cell expansion - make the volumes of adjacent cells as close as possible. So if you need to change the volume of cells for grid refinement or fitting around a non-rectangular shape, make the change gradual. (Less than 5% change per cell is a good guide)

Cell aspect ratio - make the cells as close to cubes as practical.

CFX-Build has some features which allow you to look at the quality of your mesh. On the Analysis form you can select "Visualise Mesh Quality", and it will boot CFX-Visualise and allow to check grid quality. Alternatively, you can do it under the Mesh form, under "Verify" (I think).

When doing a "real" problem, and fitting a grid to a complicated geometry, you often have to do a mesh which has a number of poor cells. Simply put, the less poor cells you have, the higher quality your mesh is, and the easier it will be to get a solution which converges. Poor meshes require lots of fiddling with under-relaxation, linear solvers and the rest to get to converge.

Regards, Glenn

Hi Zoltan,

After a bit of fiddling, and talking with some CFX support people, I have successfully used paver to mesh 2-dimensional unstructured surfaces.

This is how CFX-Support explains it:

"You should paver mesh the surfaces, which may be trimmed, with quad4 elements. You then do Sweep/Element/Extrude (for example) to generate hex elements. On the Analysis form, it is necessary to toggle on Reblock in VOLMSH, click on 3D Mesh Elements and in the popup which appears, select all the elements for the List of hexahedral elements. You should not enter anything in the Solids for VOLMSH listbox.

"VOLMSH then reads the unstructured finite element data and builds a block structure to accommodate them."

It is also possible to combine structured and unstructured mesh by using isomesh to mesh the structured part and using paver to mesh to unstructured part. On the analysis form, choose the unstructured 3D hexahedral elements for the 3D mesh elements, and the structured solids in the "Solids to mesh" box. A useful trick.

Regards, Glenn