Background

Finite Element Method

Except for a very limited number of simple problems such as beam and column elements, design by hand calculation methods is difficult to undertake. The finite element method is often required to handle complex geometric and material configurations. Finite element analysis is a numerical method for analysing complex structural and thermal problems. The technique can readily be used to assess the structural behaviour of complex components manufactured from anisotropic composite materials. Most commercial FE packages have a range of tools to facilitate the analysis of composite structures. In particular, most pre- and post-processor packages have facilities to aid the definition of laminates and enable the extraction of results at a ply level. In principle, the analysis of composite components is virtually identical to that of metal components, with the only differences being the increased complexity of the material model and, in some cases, the use of specialised elements. Before commencing the FE analysis, the objective should be established. This may determine whether a linear analysis will be sufficient for the purpose or whether a full non-linear analysis (including material and geometric non-linearity) will be required.

In common with any other finite element analysis, a mesh must be set up by defining the node co-ordinates, onto which is mapped the element topology and any other relevant geometrical data e.g. curvature of shells. A wide variety of elements are available in most commercial FE packages, most of which have some degree of orthotropic capability, in addition many packages include specialised "composite" elements, which simplify the analysis of laminated structures.

The two principal forms of specialised element for the analysis of composite structures are the laminated shell element and the laminated brick element. The laminated shell element is used for flat or curved structures whose thickness is small in comparison with the overall dimensions of the structure. For thicker structures, where inter-lamina shear stresses are significant and may lead to delamination, a separate "thick shell" formulation of the element is provided, which uses rotational degrees of freedom to represent changes in slope of the shell. Finally for thick composite structures, many FEA packages now include laminated formulations of 3D solid elements.

Unlike conventional homogeneous isotropic elements where only a single material definition is required, and in the case of shell elements a shell thickness, a laminated element must be defined in terms of its laminate structure; i.e. the thickness of each ply, its orientation and the lamina properties. Care must be taken to ensure that, when entering the fibre directions, the correct datum is used; this may be a global direction or a direction local to each element. Where the laminate structure is different for each element, or where the curvature of the shell is such that the orientation must be separately defined for each element, this may involve the preparation of a very large amount of data. The integration of FE models with braid or drape models can render this otherwise intractable task feasible.

In complex filament-wound structures, the lamination sequence can be indeterminate, where the sequence alternates over the component surface. In general, however, no attempt is made to model this effect. A more serious problem is that ply drop-offs often occur (see figure below), making it difficult to keep track of the behaviour of a given ply. Some pre- and post-processors now enable specific plies to be given unique identifiers independent of their actual position within the laminate, and their results viewed over their whole extent. The availability of additional features (e.g. tied slidelines) to join otherwise incompatibly meshed regions aids in the modelling of complex ply architectures, although mesh generation remains non-trivial.

In general, it is good practice to take advantage of symmetry in the component and thus save computer effort (data preparation and run time). With anisotropic materials, however it is not possible to simply consider the macro geometric symmetry since an apparently symmetrical structure may well behave in a non-symmetric or skew-symmetric manner, resulting in an incorrect solution. This is demonstrated in the figure below on a trivial component: a ring with helical fibres (a); if modelled using symmetry following normal engineering practice (b) will cause the model to represent a component with incorrect fibre structure (c). In many real composite structures, however, the effects of this material asymmetry is likely to be small, thus symmetry can often still be utilised to simplify the model, but much more thought is needed.

Further care must be taken to ensure that the necessary degrees of freedom exist to model a composite structure. For example, whilst a rotationally symmetric structure will always deform in a rotationally symmetric manner, if it is made from an off-axis (i.e. helical-oriented) orthotropic material, there will be a helical or twisting mode of deformation (Fig. below) which requires suitable degrees of freedom to avoid the application of an artificial constraint. In practice this means that nominally axisymmetric analyses can require additional (out-of-radial-plane) degrees of freedom to obtain meaningful results.

An important consideration is interlaminar shear stress, which may manifest itself as singularities at the edges of angle-ply panels and around holes, etc. Most element formulations will be unable to model this effect, which could potentially lead to delamination.

It is in the definition of the material model where the analysis of composites differs from more conventional analyses. It is normal for an orthotropic material model to be assumed, and the material properties may be entered in various forms, depending on the element used. For 2D in-plane and thin shell problems, only values for the Engineering constants E₁, E₂ n ₁₂, and G₁₂ are required. For models using thick shell elements, values for the through thickness shear modulus of the laminate, G₂₃ and G₃₁ are required in addition. For 3-D problems, however, a complete set of engineering constants is required, namely E₁ E₂ E₃, n ₁₂, n ₂₃, n ₃₁, G₁₂, G₂₃ and G₃₁. Alternatively the material behaviour can be defined using the nine independent constants of the 6 x 6 matrix defining the material’s compliance or stiffness matrix.

Finite element packages which include some or all of the features described above include:

ABAQUS

The ABAQUS suite of engineering analysis software packages is used throughout the world to simulate the physical response of structures and solid bodies to load, temperature, contact, impact, and other environmental conditions.

Algor
General-purpose, low cost finite element package with composite elements.

ANSYS
A general finite element package comparable in capabilities to NASTRAN. Most online info is in PDF format.

Dyna3d

Explicit finite element code with ability to model post-fracture behaviour.

I-DEAS
Full-featured CAD system from SDRC, including built-in FEA (or use as a pre-/post-processor for other systems). Powerful laminates module.

LUSAS

LUSAS finite element analysis software products can solve all types of linear and nonlinear stress, dynamics, composite and thermal engineering analysis problem...

MSC/NASTRAN
Probably the best-known of the NASTRANs, running on everything from PCs to CRAYs. There are several case studies on the site.

MSC/PATRAN
MSC's pre- and post-processor compatible with several codes, which includes a laminate modeler module.

NISA/DISPLAY
General-purpose finite element package and pre-/post-processor. Includes composites module.

Solid Edge

General purpose 3D design package

Keywords: Finite Element Analysis (FEA), composite, orthotropic, symmetry, Engineering Constants, Laminate shell elements, Thick-laminate shell elements, Laminated brick elements