The Contour panel in HyperView has contour options for FEA
results.
The following options on the Contour panel are applied to the model when you click
Apply.
- Result type
- 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. An "IP"
suffix on the result type name indicates integration point results; no "IP" suffix
indicates extrapolated results to the element corner nodes. Global element results are
with respect to the global coordinate system and are prefixed with "Global". For a
full description of global results, see Tensor Results.
- (t)
- Indicates a tensor-type result, such as stress or strain tensors.
- (v)
- Indicates a vector-type result, such as displacement, velocity, and
acceleration.
- (s)
- Indicates a scalar-type result. The components and invariants are read
directly from the ODB file.
- (c)
- Indicates complex results.
- 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.
- S-Stress components (s)
- Mises, Max Principal, Mid Principal, Min Principal, Tresca, Press, Inv3, S11,
S22, S33, S12, S13, or S23
- S-Stress components IP (s)
- Mises, Max Principal, Mid Principal, Min Principal, Tresca, Press, Inv3, S11,
S22, S33, S12, S13, or S23
- S-Global-stress components (t)
- vonMises, P1 (major), P2 (mid), P3 (minor), Pressure, MaxShear, Intensity,
In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, or XZ
- S-Global-stress components IP (t)
- vonMises, P1 (major), P2 (mid), P3 (minor), Pressure, MaxShear, Intensity,
In-plane P1 (major), In-plane P2 (minor), XX, YY, ZZ, XY, YZ, or XZ
- Displacement (v)
- Mag, X, Y, or Z
- UR-Rotational displacement (v)
- Mag, X, Y, or Z
- Entity with layers
- The Entity with layers option allows you to display a contour for a specified
element layer or section point along the thickness of the shell. 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.
- The options that control how layers will be displayed are:
- Max
- Displays the maximum value among the layers for each entity, that is maximum
tensile stress or minimum compressive stress.
- Min
- Displays the minimum value among the layers for each entity.
- Extreme
- Displays the maximum absolute values among the layers for each entity.
- Section Point 1 (SNEG, bottom)
- Results on layer 1 of the shell elements.
- Section Point 5 (SPOS, top)
- Results on layer 5 of the shell elements.
-
Note: Section Point 1 (bottom) and Section Point 5 (top) are always defined by
default. HyperView supports all layers defined in the
ODB file.
- For example:
- Element 1 Lower = -20, Upper = 10
- Element 2 Lower = -5, Upper = 30
- Lower layer:
- Legend Max = -5, Min = -20
- Upper layer:
- Legend Max = 30, Min = 10
- Min layer:
- Legend Max = -5, Min = -20
- Max layer:
- Legend Max = 30, Min = 10
- Extreme layer:
- Legend Max = 30, Min = -20
- 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.
- The Abaqus ODB reader supports element results at
POSITION=INTEGRATION POINTS (default), NODES, and CENTROIDAL. The ODB file does not
support AVERAGED AT NODES. Abaqus ODB always has results
for integration points regardless of the position parameter setting in the output
request.
- HyperView supports these results with respect to the
Display corner data option as follows:
- Without "IP" suffix
- For example: S-Stress components (s)
- Display corner data on is the integration point
results are extrapolated to the element corners. This is equivalent to
POSITION=NODES in Abaqus.
- Display corner data off is the integration point
results are averaged as the base result of the element. This is equivalent
to POSITION=CENTROIDAL in Abaqus.
- With "IP" suffix
-
- Display corner data on is the integration point
results are displayed at the nearest element corners.
- Display corner data off is the integration point
results are averaged as the base result of the element.
- Refer to 1st-Order Elements and 2nd-Order Elements for schematics describing this information.
Also refer to 1D Elements.
- 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.
- The Abaqus part is written according to the guidelines
described in Supported Tensor Results.
- 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).
- Elemental System
- Transforms results to the elemental coordinate system. In HyperView, the elemental coordinate system is defined by
element connectivity, which differs from the Abaqus
elemental system, but is similar to the Nastran
elemental system.
- Analysis System
- Transforms the results to systems associated with each elements as they are
defined in the result file. Because every result in Abaqus has its own system that can change with time, the
results can not be populated as a HyperView analysis
system. Therefore, the analysis system option is not applicable to Abaqus results and is equivalent to the global system.
- 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).
- Projection Rule
- Abaqus uses X as the primary axis and Z as the secondary
axis.
- Averaging Method
- No averaging method is used. Color will be displayed in element-based results, a
solid color for centroidal results, or multiple color bands within an element.
- None
- Simple
- Tensor and vector components are extracted and the invariants are computed
prior to averaging.
- This option is equivalent to the Abaqus/Viewer
"compute scalars before averaging" option
- Advanced
- Tensor or vector results are transformed into a consistent system and then
each component is averaged separately to obtain an average tensor or vector. The
invariants are calculated from this averaged tensor or vector.
- This option is similar to the Abaqus/Viewer
"compute scalars after averaging" option.
- Difference
- The difference between the maximum and minimum corner results at a node.
- Use variation (%)
- The relative difference at a node from corresponding corner values with
respect to the value range from all nodes in the selected components.
- This option is equivalent to the "averaging threshold (%)" option in Abaqus/Viewer, but the HyperView denominator is different.
The following options are automatically applied to the model as you enter information:
- Display options
- The display options change the appearance of the contour colors.
- Discrete color
- Produces discrete color bands on contour plots with distinct boundaries
between contour levels. This option uses a texture mapping capability in your
graphics card. If your graphics card does not support texture mapping, the
performance may slow down.
- Show feature lines
- Display feature lines for the displayed components. You can set the desired
feature angle from the Tools menu, Options dialog, Visualization tab.
- Interpolate colors
- Interpolates the contour colors from the undeformed shape (with a zero value)
to the result variable reported from the solver. If you do not select
Interpolate colors, the contour colors remain the same for all frames. This is
only applied to modal and static animation.
- Legend threshold
-
- Max
- Enter the value to be assigned to the highest color in the contour plot.
Activate the Max check box to apply the value.
- The new value is also changed in the Values section of the Edit Legend
dialog.
- If a value entered for threshold Max is invalid, it will not be applied and
the panel will be updated to reflect the actual state.
- Min
- Enter the value to be assigned to the lowest color in the contour plot.
Activate the Min check box to apply the value.
- The new value is also changed in the Values section of the Edit Legend
dialog.
- If a value entered for threshold Min is invalid, it will not be applied and
the panel will be updated to reflect the actual state.
- Multiplier
- Enter the multiplier for scaling all the result values.
- Edit Legend
- Opens the Edit Legend dialog where you can change the legend
properties.
- Result display control
- The following options allow you to manage the result display.
- Overlay result display
- Overlays contour, tensor, and vector results in the same window. If all
results are displayed simultaneously, available memory may be affected.
- Clear Contour
- Clears the contour and returns the model to its original state.
- Query Results
- Opens the Query panel where you can view and export properties and other information
related to nodes, elements, components, and systems contained in the active model.
