Composite modelling with solid elements 1

[WillBerg]

Hello,

is there any FEM Software/System capable of:

1.meshing directionally reinforced composites with tetrahedrals or 8(20)-node bricks (and calculating elastic properties of every resulting element);
2.calculating the above structure;
3.analyzing the results in relation to composite failure criterions or evaluating the actual stresses in the structural components of composite;
4.other technique considering non-unidirectonal (but also not random) fiber reinforcement layers;
5.Any of 1., 3. or 4.?

Thanks.

 

[Erik Panos Kostson]

As you probably know composites are normally modelled with shell (layered elements) or continuum shell elements.
(Very often for shell modelling of composite structure a composite laminate module is used to define the material properties, and then to derive the CBD matrices that are often used and can go into the global stiffness of the FEA model. This derivation is often based on classical laminate shell theory and not 3D theory)

There are though situations when 3D modelling of composites might be necessary, because classical laminate shell theory is not adequate.

An example of such a case is if the through thickness stresses are high/important and need to be captured accurately.

For such a case, commonly used general purpose FEA software have some elements called composite solid elements (layered 3D hex-elements, e.g., with 8 or 20 nodes), that can capture such a situation perhaps more accurately.

If you search for this element on the internet you will get a lot of information.

Hope this helps.

 

[rb1957]

I think it's more common to use plates and laminate properties to model each ply.

You can model individual plies and resin or lump plies (in different directions) using a laminate property card.

another day in paradise, or is paradise one day closer ?

 

[jotunn]

Definitely agree with the others that 2D elements are more common.

That said, a few years back I had a project where 3D composite elements were better suited. I was using Femap as the pre/post and NeiNastran as the solver (this was before Autodesk purchased NEI and subsequently neutered the program in typical Autodesk fashion). It worked decently...with some limitations.

Limitations being:
-Have to manually edit the MAT12 card to input allowables (will not come out of femap)
-Allowables must be in stress format, even with a strain solution (better documentation needed)
-Have to add the PCOMP ID to the PSOLID card manually
-Changing element orientation (solid element...first edge) doesn't seem to be possible in Femap (so you have to be very careful how they're defined/meshed).

 

[RPstress]

You can put properties in if you know them (most test programs find adequate through-thickness stiffnesses and strengths). However, you will have a problem finding adequate failure criteria accounting for both inplane and through-thickness forces at the same time. Combinations of inplane stresses are bad enough but couple those with high out-of-plane ones and it's usually guesswork. Full 3D failure criteria do exist but they aren't very accurate. Good luck with your Googling.

 

[ESPcomposites]

Yes, FEA can do all of those things.

However, from an engineering perspective, the question is how can FEA be useful for composites? Lets split that in two parts:

- Deformations
For the most part, FEA can be used to accurately determine the deformation of composite structures. This includes problems such as elastic stability and natural frequency. 2D elements are usually suitable for this. In some cases, you may be interested in the effects of transverse shear stiffness. 3D elements may be considered for such a case.

- Strength
FEA can be used to determine strains/stress in composite parts (2D or 3D). BUT, for practical scenarios such as a holes, joints, impact damage, etc., there is no well-accepted failure criteria that works in 3D (and those scenarios must consider 3D to be accurate). Instead, we use semi-empirical approaches. For some scenarios, FEA can then be useful when combined with test data. But each method is going to be a specific "recipe" since it is semi-empirical. For these methods, we usually use 2D elements since we have already accepted that predictive shortcomings must be compensated with test data (so why build a 3D model at that point). We can not currently create a 3D FEM, extract the strains/stress, and predict failure for the practical scenarios of interest.

Note that "pure" strength prediction via 3D FEM is still an ongoing research topic. For the "simple" case of a laminate with a hole, we would need to predict localized subcritical failures in 3D (a nonlinear problem). In general, there are many damage mechanisms and it is a complex problem (also the reason it has not been solved). There are some attempts such as SIFT for that. For delamination problems, ILFM (interlaminar fracture mechanics) is an option, but is still gaining acceptance for general use.


Brian

http://www.espcomposites.com