Finite element meshing

[longisland]

Hi all,

I would like to know the difference between a triangular mesh & an irregular shape mesh in FEA analysis. What are the limitations & advantages between the two approaches?

Thanks

 

[fetraining]

longisland,

a triangular shaped element with three nodes will generally have an inferior performance to a quadrlateral shaped element with four nodes. This manifests itself in poor internal mappping of the stress distribution in stress gradient regions and a tendancy to be over stiff. Different FE codes exhbit this to a more or less extent.

The first choice in meshing would always be a very regular shaped quadrilateral mesh. The 'perfect' quad is square. The 'perfect' triangle element is an equilateral triangle. As soon as the quad or triangle is distorted errors start to creep in.

Most real life shapes mean it is tough to have an all quad or very regular quad mesh. So an irregular quad mesh is usually produced. It may also have triangular elements to allow mesh refinemnt around various features, or to deal with triangular shaped features such as fillet run out.

This is quite standard and should give reasonable results as long as the distortion of each element is within limits. Most preprocessors will give yu a map of the main distortion parameters so that you can check the 'goodness' of your mesh.

The only time I use a purely triangular mesh is if there are very large amounts of double curvature and I can't use higher order elements and the mesh needs to be coarse. The 3 noded trangle fits the surface accuratly. It is not a nice solution, but it avoids using planar quad elements which fit themselves to curved surfaces by internal rigid links between the flat element surface and the curved surface.

The whole art of meshing is very subjective, but if you keep an eye on the distortion parameters, do convergence checks and look at unaveraged stresses for bad stress distributions then you should be ok.

regards,

Tony

 

[GregLocock]

I'd add that it also depends on what you want from your analysis. I'm often only interested in the resonant frequencies, so local stresses don't matter. So even an ugly mesh in some details will have no effect on the overall stiffness of the part. Our errors are more likely to be bad mass estimates for other parts than some niggling changes in stiffness of the meshed part.



Cheers

Greg Locock

SIGlease see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[longisland]

Hi,

Thanks for the feedback

 

[mtnengr]

The above discussions are relevant. Just to put a cap on this thread, I would like to add the following: The correct mesh distribution has to deal with the order of the displacement function being assumed and the method of numerical integration being used.

In the early development of FEM, triangular elements were used, even for quads (four internal triangular elements with a central point at its CG). Five points were then the major points of interest. As the order increased, iso-parametric methods became popular which allowed more points (7, 9 and 16 points were typical) of interest to be considered, but yet swept out of the final stiffness formulation when establishing displacements.

Some planar mesh generators strictly use the triangular mesh and correct its distribution using an energy function. For three-dimensional problems often the tetrahedron is used as the primary building block element. The same distribution rules apply.

So, you have to understand the basic assumptions of the finite element and its distortion rules. Stress distributions or velocity gradients in CFD require localized fineness whereas that is not the case for dynamic (frequency) determinations.