Using the Contour Panel for ANSYS Results

HyperView supports ANSYS elemental results (PLESOL) and nodal results (PLNSOL).

The procedures and setting required for obtaining these results are described below.

The Contour panel in HyperView has contour options for FEA results. The following overview focuses on ANSYS .rst and .cdb files. For details of other common options, refer to the HyperView Contour panel online help topic.

HyperView can display ANSYS results as continuous contours or discontinuous element contours.
Option Description
Result type The Result type section allows you to select the result type and the corresponding component type that should be used to calculate contours. Use the first drop-down menu under Result type to select one of the available result types.
The options change depending on the currently loaded result file. Each result type is followed by a letter that indicates the category to which it belongs.
(v)
Indicates a vector-type result, such as displacement, velocity, and acceleration.
(t)
Indicates a tensor-type result, such as stress or strain tensors.
(s)
Indicates a scalar-type result.
  The second drop-down menu in the Result type section allows you to choose the data component type. The list of available components is based on the selected result type.
The Mag option is equivalent to the summation plot of displacements in ANSYS.
Displacement (v)
Mag, X, Y, Z
Reaction force (v)
Mag, X, Y, Z
Creep strain (t)
vonMises, P1(major), P2(mid), P3(minor), Pressure, MaxShear, Intensity, In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, ZX
Elastic strain (t)
vonMises, P1(major), P2(mid), P3(minor), Pressure, MaxShear, Intensity, In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, ZX
Plastic strain (t)
vonMises, P1(major), P2(mid), P3(minor), Pressure, MaxShear, Intensity, In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, ZX
Stress (t)
vonMises, P1(major), P2(mid), P3(minor), Pressure, MaxShear, Intensity, In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, ZX
Thermal strain (t)
vonMises, P1(major), P2(mid), P3(minor), Pressure, MaxShear, Intensity, In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, ZX
Direct vonMises strain (s)
Elastic, Plastic, Creep, Thermal
Energy (s)
Plastic work, Plastic state variable, strain energy, kinetic energy
Geometry (s)
Element volume
Nonlinear (s)
Equivalent plastic stress, Stress state ratio, Hydrostatic pressure, Equivalent plastic strain
Porosity (s)
NPOR (porosity due to void nucleation), TPOR (total porosity - Gurson material model), GPOR (porosity due to void growth)
Swelling strain (s)
Scalar value
Entity with layers Allows you to display a contour for a specified element layer when a layer definition is available for an element. The contour will be applied to all layers defined in the model. If an element has no layer definition, as in a mass or solid, the contour is also displayed regardless of which layer is selected.

For ANSYS results, select Upper or Lower.
Use corner data If corner data is available, the Use corner data option is enabled. If you activate the option, HyperView displays color bands by interpolating available corner results within each element. A discontinuity of the result distribution across element boundaries can be seen.

ANSYS elemental results are available at the corners of elements. Therefore, this option should always be selected for both elemental and nodal solutions while working with ANSYS *.rst and *.rth result files.
Selection Before creating a contour plot, you must pick one or more entities from the model. You can do this by picking entities directly from the screen, using the quick window selection, or clicking the Elements or Components input collector and using the extended entity selection menu. If no selection is made, the contour will be applied to displayed components or elements by default.
Resolved in The Resolved in drop-down menu allows you to select the result coordinate system to be used to contour the results. The available options are dependent on the current selection for Averaging method. You can select the analysis, elemental, or global coordinate system as well as a user-defined system. The System input collector is enabled when User System is selected.
  Global System Transforms to the global system.
(proj: none)
Indicates that no projection rule is selected for shells. When a projection rule is selected (using the Projection Rule… button) it is displayed, for example, (proj: y, x).
  User System Transforms the results to a user-defined coordinate system.
This option is available when the results or model file contains a user-defined coordinate system. Click the System input collector to select a system by ID or pick from the screen.
(proj: none)
Indicates that no projection rule is selected for shells. When a projection rule is selected (using the Projection Rule… button) it is displayed, for example, (proj: y, x).
Averaging method For ANSYS results:
  • For element solutions (PLESOL), set the Averaging method to none.
  • For nodal average results (PLNSOL), set the Averaging method to advanced.
  • For Direct von Mises results for nodal averaging, set the Averaging method to none.
  • For nodal average results, do not check the Use variation [%] check box under the Averaging method field.
  • When the Use variation [%] check box is selected, type a value of 100 for 100% variation.

Color will be displayed in element-based results, a solid color for centroidal results, or multiple color bands within an element.
Projection Rule ANSYS does not use any projection rules for element results. Set this option to none while plotting.