The computations necessary to display results stored in the output database depend on whether the results are for a node-based quantity, such as displacement or velocity, or for an element-based quantity, such as stress or strain.
How node-based field output results are computed
Node-based field output variables are written to the output database at each node, along with any nodal transformations applied during model creation. For the display of nodal field output variables, ABAQUS/CAE reads the required values from the output database for each node included in the plot. By default, these values are displayed in the global coordinate system; you can choose to apply the nodal transformations to the results or to apply a user-specified coordinate system transformation. The final values are then used to produce contours, nodal probe values, display groups or color coding based on results, or X–Y data along a path.
How element-based field output results are computed
Element-based field output variables are written to the output database at the integration points, the element centroid, or the element nodes, depending on the variable. For the display of element-based field output variables, ABAQUS/CAE reads values from the output database for all elements connected to all nodes included in the plot. Computations are then applied to these values to produce contours, nodal probe results, display groups or color coding based on results, or X–Y data along a path.
For results saved to the output database at the integration points or at the element centroid, the first computation applied is extrapolation. (Results saved at the element nodes do not require extrapolation.) For contour plots only, you can choose quilt-type extrapolation, in which case the remaining computations discussed below do not apply. To learn more about quilt-type extrapolation, see “Understanding how contour values are computed,” Section 26.1.1. For all other methods of results display, ABAQUS/CAE extrapolates results to the nodes using weighting appropriate for the element type and shape.
Extrapolated values are generally not as accurate as the values calculated at the integration points. Therefore, adequately detailed meshing is recommended around nodes where accurate nodal values of such element results are needed. You should be particularly careful interpreting output variables extrapolated to the nodes for second-order elements with midside nodes outside the quarter-point region, such as when one edge is collapsed in two dimensions or one face is collapsed in three dimensions.
Extrapolation of element tensor quantities is performed on the individual tensor components in the local material coordinate system. Nodes common to two or more elements receive extrapolated values from all contributing elements. Depending on the characteristics of your model, these contributions may originate from more than one result region. If all contributions at a node originate from a single result region, the values are combined as necessary in further computations. If contributions are received from more than one result region, you can choose to respect the region boundary and keep the contributions separate in further computations or to ignore the region boundary and combine the values. The default result regions in an output database duplicate the regions that were used to assign section properties to the model prior to analysis. Alternatively, you can select element sets or display groups to use as result regions. For more information, see “Controlling computations at region boundaries,” Section 24.5.7.
If invariants or components are requested, you can specify whether ABAQUS/CAE should use the extrapolated data from each element or the combined data from all contributing elements to compute the invariants. By default, invariants are computed before the extrapolated results are combined (averaged). Contour plots of invariants or components may be affected by the order in which ABAQUS performs the computations. For example, values for the von Mises stress may exceed the yield stress of inelastic materials; in addition, the invariant results may not take into account situations where the material orientations vary within a finite element in a non-isoparametric fashion. If invariants are computed after averaging, ABAQUS determines the orientations at a node by averaging the contributing element orientations; component values will be affected if the orientations differ between contributing elements.
If you select element sets to define the result regions and invariants will be computed after averaging, the element sets that you select must contain compatible elements. Compatible elements
share the same basic element type (continuum, shell, beam, etc.),
use interpolation functions of the same order (first-order elements versus second-order elements), and
have the same integration scheme (reduced integration, full integration, etc.).
Finally, computations depend on whether you choose to display the field output values or discontinuities; discontinuities are the differences in field output values between adjacent elements.
Field Output: For the display of field output values, the calculated invariants or components at nodes common to two or more elements are averaged conditionally, depending on the compatibility of contributing result regions and on options you select. For more information, see “Understanding result value averaging,” Section 24.5.2.
Discontinuities: For the display of discontinuities, the calculated invariants or components at nodes common to two or more elements are compared to determine the greatest difference, depending on the compatibility of contributing result regions and on options you select. Nodes associated with only one element and nodes receiving equivalent values from all contributing elements will show a value of zero in a plot of discontinuities.
How result transformations are computed
Both node- and element-based results can be transformed into a user-specified coordinate system; see “Transforming results into a new coordinate system,” Section 24.5.8, for information on applying a transformation to your results.
Element-based results for three-dimensional continuum elements and all node-based results are transformed into the specified coordinate system based on the locations of the results. The 1-, 2-, and 3-directions for the transformed results correspond to the X-, Y-, and Z-directions of a rectangular coordinate system; the R-, 
-, and Z-directions of a cylindrical coordinate system; and the R-, -, and 
-directions of a spherical coordinate system.
Element-based results for two-dimensional continuum elements, shell elements, and membrane elements are transformed by rotating the results about the element normal at the element result location. The 2-direction for the transformed results is determined by the projection of the rectangular Y-direction or the cylindrical or spherical -direction onto the element plane. If the projected coordinate system axis and the element normal form an angle less than 30°, the next axis is used instead and a warning message is displayed. This method of results transformation is slightly different from the method used by ABAQUS/Standard and ABAQUS/Explicit to compute local orientations (see “Orientations,” Section 2.2.5 of the ABAQUS Analysis User's Manual).
Element-based results for beam and truss elements cannot be transformed; they are always displayed in the local element orientation system. In addition, element results for rebar and for CAXA, SAX, or SAXA elements are not transformed.
When you transform results to a user-specified coordinate system, you can also adjust the results to account for the rigid body transformation of the coordinate system. You can adjust the display of primary variable results, deformed variable results, or results from both variables.