Engineering analysis + design software

User Area > Advice

Finite Element Equilibrium

In terms of finite element equilibrium, there are two important properties that are always satisfied by the finite element solution using either a coarse or a fine mesh. To describe these properties consider the following portion of a mesh under the application of an arbitrary force, the four elements (1,2,3,4) share the same node (i).

The following diagram, representing an exploded view of these four elements, shows the forces obtained at the nodal position (i) and those on element (2).

The two properties may now be defined as

         Nodal point equilibrium: At any node, the sum of the internal element point forces is in equilibrium with any external loads that are applied to the node. The internal forces include the effects due to body forces, surface tractions, initial stresses, concentrated loads, inertia and damping forces, and reactions. Thus, for an externally non-loaded node in a linear static analysis, such a summation will be zero.

         Element equilibrium: Each element is in equilibrium under its internal forces

Nonlinear analyses may produce out-of-balance residual forces at a node, depending on the degree of convergence obtained during the solution. For a well-converged solution, however, these are insignificant. See nonlinear iterative strategy for more information.

Although nodal and element equilibrium is achieved as described above, in a general finite element analysis, differential equilibrium (e.g. stress equilibrium) is not necessarily achieved at all points of the continuum considered – most notably at the shared boundaries of elements. The reason is as follows…

In the displacement-based finite element method, a C0 continuous approximation for the displacements is assumed within each element. This means that the displacements at any point in a mesh will be continuous and ensures that no gaps appear between elements. The element stresses are calculated using derivatives of the displacement which means that they will not necessarily be continuous and give rise to inter-element discontinuities or “jumps” in stress between adjacent elements (an example is given in “Implication: Linear Versus Quadratic Elements?”). This is particularly the case for coarse element meshes. The discontinuities at adjacent element boundaries are reduced with mesh refinement and the rate at which mesh refinement reduces such discontinuities is determined by the order of the elements in the mesh – higher order elements converging faster than low order.

For the same reasons that element stresses are not continuous across element boundaries, the element stresses at the surface of a finite element model are, in general, not in equilibrium with the external applied tractions. Again, this effect is minimised with mesh refinement.

Experience has shown that the most accurate locations for stress output are the Gauss points. Nodal points, which are the most accessible, are actually the worst output location for stresses. Reasons have been given above, but include the fact that shape functions tend to behave badly at element extremities and it is reasonable to expect that the shape function derivatives (i.e. strains/stresses) sampled in the interior of the element would be more accurate than those sampled at the periphery of the element.

This evokes the question of how to obtain accurate stress results from a finite element model?

Implication:  Smoothed or Unsmoothed Stress Contours?

One method for obtaining reasonable nodal stress output is by extrapolating the “exact” stresses at Gauss points to the nodal positions using the element shape functions. Consider the following diagram, representing the same exploded view of the four elements shown earlier.

For element 2, the nodal stresses at nodes (1,2,3,4) are obtained by

  • Defining a fictitious element (shown by the dashed lines) with nodes at the element Gauss points (a,b,c,d)
  • Extrapolating the Gauss point stresses to the nodal points of the real element (1,2,3,4) using the displacement shape functions of the fictitious element, i.e.

Where N is the number of Gauss points, and subscripts i and I denote nodal and Gauss point values respectively.

The accuracy of the extrapolation procedure is dependent on both the presence of a reasonably uniform stress field and the type of shape function used in the element chosen. For instance, a high stress gradient across an element would be more likely to extrapolate incorrectly, particularly if a linear shape function element is being used.

This procedure is carried out for the other elements and the nodal stresses at the common node (i) are obtained as (si)1, (si)2, etc. As pointed out above, these stresses are not usually equal and a single “averaged” or “smoothed” nodal stress value is obtained using

When this procedure is carried out for all nodes in an element assembly, the ensuing averaged stress values provide a reasonable approximation to a continuous stress field. This is a straightforward and economic solution and works well on the whole. See later for more details on the circumstances that smoothing should not be used. This is the default method used in MODELLER when smoothed results are selected in the contour layer properties. If smoothed results are not selected then the extrapolation procedure is still performed, but the averaging process is omitted. The averaging procedure is also carried out when the "values" and "loading" layers are selected.

Note that, for shell elements, the local Gauss point stresses and strains are transformed to global stresses and strains before extrapolation to the nodes. The mean global stresses are then transformed to the local shell system at the nodal point before evaluation of the nodal stress resultants.

Other methods are available, based on a least squares fit over the integration point stress values of the elements. The least squares procedure might be applied over the patches of adjacent elements or even globally over a whole mesh. However, if the domain over which the least squares fit is applied involves many stress points, the solution will be expensive and, in addition, a large error in one part of the domain may affect rather strongly the least squares prediction in the other parts.

In general, it is recommended to display unsmoothed stress contours at an early point during the processing of results. In this way, severe stress discontinuities between elements will be apparent and the possible requirement of mesh refinement and/or the use of higher order elements may be considered.

In areas of interest where the stress results will be used in the design process, smoothed contours would ideally be similar to unsmoothed contours. The inference from this being that a smooth stress transition across the element boundaries indicates that the stress distribution in the structure is being simulated sufficiently accurately. For sections of the model that are not of interest, a coarser mesh would normally be used and such a comparison in these areas would typically give significantly different contours - smoothed contours appearing more like a patchwork quilt!

The nodal averaging technique is sufficiently robust that such stress values will tend to be pretty much those that would be obtained at the same location with mesh refinement – as long as the element mesh is reasonably uniform.

At all times, it is imperative to remember that the finite element method is an approximate numerical technique (albeit a good one!) and that smoothed stress results can give good results but need careful attention.

Implication:  Limitations of the averaging scheme

In addition to taking no account of the size of the adjacent elements, the averaging method must not be used

  • At mesh locations in which geometric or material properties change.

  • For local or global stress output for shell elements that are non-planar. At the intersection of the three elements shown below, for instance, it is invalid to add the local sy stresses.

  • Interconnecting BEAM or GRIL elements. It is necessary to use the advanced selection facility to extract results for longitudinal members and transverse members separately.

Consider the situation in which Mx results have been selected for display using the “values” layer in MODELLER and both transverse and longitudinal members are active. The averaged value displayed at the central node number (1) will be comprised of the local Mx values from the two longitudinal and two transverse members that connect to this node. It must be noted that the Mx values are local to the elements (as shown in the diagram), so that the Mx values for the longitudinal members act at 90 degrees to the Mx results in the transverse members. This means that the averaged values will be meaningless since the Mx results from the longitudinal members will be averaged with the Mx values of the transverse members that are acting in a completely different direction. One remedy would be to ensure that the Mx values from the longitudinal members were combined with the more appropriate My values from the transverse members – results that are acting in the same direction. This remedy is not actually workable, and so the use of the “diagrams” layer or the proper use of “advanced selection” should be invoked if the “values” or “contour” layers are actually required.

  • Selecting smoothed or unsmoothed stresses can have significant implications on the values of stress obtained. Difficulties of interpretation may result if the local axes of adjacent elements are not aligned. Consider the following two shell elements.

    In this case, averaging the sx stress components at one of the two adjoining nodes will result in a sx stress being averaged with a sy stress - the resulting smoothed stress being clearly incorrect. This may be overcome for most quadrilateral meshes by modifying the element axes (cycling or reversing the underlying feature axes). For triangular elements, however, no amount of cycling will obtain a consistent set of local element axes - as will be observed in the following figure.

    In the case of triangular elements, the stress results should be transformed appropriately. Element results that are displayed in a global axis system will not be affected by such local element axis problems.

  • Where a shell surface is curved or does not lie in one of the global axis planes (even if flat), stresses will be difficult to interpret in Modeller since the chosen stress component may "intersect" the element plane at an awkward angle. In such cases the stresses should be transformed to an orientation corresponding to the shell plane or a direction-independent stress measures such as principal or von Mises. The problem can be seen in the following diagram in which the default sx (global) direction can be seen to be at an orientation that is unlikely to be in a helpful orientation when compared to the more usual orientation of the local sx direction.

Implication:  Removal of elements affects the stress contours

  • An implication of the averaging process is that when contouring selected parts of the structure, the elements that have been removed from the active list will no longer make a contribution to the averaging process. Depending on the relative size of the stress contributions that are now missing, the contours at the selected element boundary may change significantly. Unsmoothed results do not behave in this manner.

Additional Links

Finite Element Theory Contents


innovative | flexible | trusted

LUSAS is a trademark and trading name of Finite Element Analysis Ltd. Copyright 1982 - 2022. Last modified: November 29, 2022 . Privacy policy. 
Any modelling, design and analysis capabilities described are dependent upon the LUSAS software product, version and option in use.