Results of a Finite Element Analysis

The primary results in a finite element analysis are grid point displacements and rotations.

Element results such as stresses, strains, and strain energy density are derived from those results. Other results include element forces, MPC forces, SPC forces, and grid point forces.

Results of a finite element analysis are post-processed using a graphical tool.

The definitions of the output options can be found in the I/O Options section. An overview of the result files can be found in Results Output by OptiStruct.

Information on stress, strain and force definitions regarding their coordinate system definition can be found in Element Results Representation for Models and on the respective element definitions.

Displacements

Displacements and rotations are computed in linear static, and frequency response analyses. In addition, in frequency response velocities and acceleration are computed.

Eigenvectors are the primary result in a normal modes and buckling analyses. In a normal modes analysis, they are normalized with respect to the mass matrix or with respect to the maximum vector component. In a buckling analysis, the latter always applies.

Displacements, velocities, accelerations, and eigenvectors are grid point results. They are plotted as a deformed structure, or as a contour on the undeformed structure. Some post-processors, such as HyperMesh and HyperView, also allow the animation of the displacements.

Stresses

The stresses are secondary results in a static analysis.

Stresses near notches and other sharp corners, point loads and boundary conditions, and rigid elements are often unreliable due to the singularities in these points. This is not a trait unique to OptiStruct, but is inherent in the finite element method itself. A mesh refinement in such places can improve the stress prediction. A theoretically infinite stress cannot be predicted by finite elements.

Stresses are primarily calculated at the Gauss integration points. These give the most accurate prediction. However, element stresses, corner stresses, and grid point stresses are provided.

Element stresses are calculated at the centroid of the element. They should only be post-processed using an assign plot. Contouring of element stresses vastly underestimates the extreme values due to the smearing across element boundaries.

The stresses of interest are usually found on the surface of a structure. Mesh refinement will actually not just improve the stress prediction but also change the location of the point of stress evaluation. Therefore, it is common practice to use a skin of thin membrane elements in 3D modeling, or rod elements in 2D modeling, to evaluate the stresses on element surfaces or edges, respectively. This method is accurate since it considers the correct condition of a stress-free boundary if no load is applied to the boundary. The method of skinning a model also has the advantage of much faster post-processing of solid models because only the membrane skin needs to be displayed.

Besides assign plots, elements stresses can be viewed in tensor plots that can help in the evaluation of the load path in a structure by evaluating the principal stress directions.

Corner stresses are computed by extrapolating the stresses from the Gauss points to the element grid points. Corner stresses are plotted in a contour plot. Corner stresses for solid elements are not available for normal modes analysis.

Grid point stresses are computed by averaging the corner stresses contributions of the elements meeting in a grid point. The averaging does not consider the condition of a stress-free boundary. Further, interfaces between different materials, where a stress jump normally can be observed, are not considered correctly because of the smearing of the stress. Grid point stresses are plotted in a contour plot.

For first order elements, grid point stresses do not provide higher accuracy over element stresses. For second order elements, the stress prediction might improve by using grid point stress over element stresses, considering the weaknesses mentioned above.

Strains

Strains are secondary results and are calculated as element strains.

Remarks made above on element stresses apply here too.

Equivalent Plastic Strain

Equivalent plastic strain is defined as:

ε_{p s} = \sqrt{\frac{2}{3}} \int_{0}^{t} \sqrt{{\dot{e}}_{i j}^{p l} {\dot{e}}_{i j}^{p l}} d t

Where,

$ε_{p s}$: Equivalent plastic strain.
$e_{i j}^{p l}$: Plastic strain deviator.
${\dot{e}}_{i j}^{p l}$: Rate.

It determines the length of trajectory in the 9-dimensional plastic strain space (mod-ulo the $\sqrt{\frac{2}{3}}$ factor). Here, it is assumed the indices $i, j$ range over the values 1, 2, 3, and the standard summation convention holds for the repeated indices.

Von Mises Plastic Strain

Von Mises plastic strain is defined as a measure of the plastic distortion in shape of an infinitesimal element of the medium.

ε_{M i s e s} = \sqrt{\frac{2}{3}} \sqrt{e_{i j}^{p l} e_{i j}^{p l}}

Where,

$ε_{M i s e s}$: Von Mises plastic strain.
$e_{i j}^{p l}$: Plastic strain deviator.
${\dot{e}}_{i j}^{p l}$: Rate.

Equivalent Plastic Strain versus Von Mises Plastic Strain

Generally, these two quantities are different:

ε_{p s} \neq ε_{M i s e s}

On one hand:

{\dot{ε}}_{p s} = \sqrt{\frac{2}{3}} \sqrt{{\dot{e}}_{i j}^{p l} {\dot{e}}_{i j}^{p l}}

On the other:

{\dot{ε}}_{M i s e s} = \sqrt{\frac{2}{3}} \frac{1}{2 \sqrt{e_{i^{'} j^{'}}^{p l} e_{i^{'} j^{'}}^{p l}}} (2 e_{i j}^{p l} {\dot{e}}_{i j}^{p l})

= \frac{2}{3 ε_{M i s e s}} (e_{i j}^{p l} {\dot{e}}_{i j}^{p l})

So:

\sqrt{\frac{2}{3}} \sqrt{{\dot{e}}_{i j}^{p l} {\dot{e}}_{i j}^{p l}} \neq \frac{2}{3 ε_{M i s e s}} (e_{i j}^{p l} {\dot{e}}_{i j}^{p l})

Strain Energy Densities

Strain energy densities are secondary results in static and normal modes analysis.

They are calculated as element strain energy densities. Remarks made above on element stresses apply here too.

Forces

Element forces, MPC forces, SPC forces, and grid point forces are printed as tabulated output.