When you click a part in the tree view, all the items associated with the part are selected in the display area based on the Selection Select panel. For example, if the selection method is set to elements, clicking a part in the tree view will select all the elements associated with that part. Then, any operation associated with the selection can be performed, such as Results Inquire Inquire Element Information.
|Table 1: Selecting Contact Entry in Tree View|
|Analysis Type||Contact Type|
|Bonded or Welded||Surface or Edge Contact|
|Linear||See Note 1.||Nodes connected with contact elements are selected.|
|Nonlinear||See Note 2.||Nothing is selected.|
|Thermal||See Note 1.||Nothing is selected.|
|Fluid Flow||Nothing is selected.||Not applicable.|
|Electrostatic||See Note 1.||Not applicable.|
|Mass Transfer||Nothing is selected.||Not applicable.|
When beam, plate/shell, or 2D elements are included in the analysis, the parts can be displayed or rendered as the 3D geometry instead of the line or planar geometry. This can be done by right-clicking on the heading for that part in the tree view and selecting the 3D Visualization command. Table 2 and Figure 1 provide additional details. In all cases, only the nodes and elements on the original mesh can be selected; the fictitious nodes and elements created to show the 3D shape cannot be selected. Loads and boundary conditions are shown at the original mesh.
|Table 2: 3D Visualization|
|Element Type||Applicable Analysis Type||Notes|
|Beam||Linear and Nonlinear||Cross section shown with 3-D visualization. Beam elements can only be visualized if the cross-sectional properties were defined using the AISC 2001 or 2005 cross-section library or using one of the pre-defined User Defined shapes (wide flange beam, channel, and so on).|
|Plate or Shell||Linear and Nonlinear||Thickness shown with 3-D visualization.|
|2-D axisymmetric||all||Cross section shown revolved around the Z axis with 3-D visualization.|
|2-D planar||all||Thickness in -X direction shown with 3-D visualization.|
(a) Beam element with loads. A beam element mesh is simply a straight line; the cross sectional properties are treated analytically.
(b) With 3D Visualization active, the actual cross sectional shape is shown. Note how the loads are still shown on the original elements.
(c) 2D axisymmetric model. Analytically, the analysis treats the model as if revolved around the Z axis.
(d) With 3D Visualization active, the 2D mesh and results are shown in their 3D form. The results are the same around the perimeter, so vector results are interpreted as being relative to the Z axis. For example, a true representation of the Y displacement would show a positive value on one side of the model and a negative value on the opposite side. Instead, the Y displacement should be interpreted as the displacement component away from the rotation axis. (A better suggestion is for you to create a cylindrical coordinate system and view the results in terms of radial, tangential, and axial. See the page Setting Up and Performing the Analysis:.)
|Figure 1: Examples of 3D Visualization|
The Presentations branch of the tree view contains the different views for the current model. The thing to keep in mind is that each presentation is a separate window. To switch between the different presentations/windows, either click the presentation's name in the tree view or use the Window pull-down menu and choose the appropriate window. To close a presentation, switch to it and click the X to close the window.
The name of the presentation (shown in the tree view and in the window's title bar) only represents the name when the window was created. By using the pull-down menus, the displayed result can be set to anything. Thus, the default Stress presentation may actually be showing a displacement result when changed.
Once a presentation/window is set up with special settings that you want to save for future use, right-click the presentation name in the tree view and choose either Save with Model or Save with System.
Any model can be mirrored about a maximum of three planes. This is most often used in a symmetry analysis to create a display of the full model. For example, Figure 2 shows the analysis of a symmetric frame. A full display is created in the Results environment to show the complete frame for the report.
(a) This is the complete model that was analyzed. The analyst took advantage of symmetry and analyzed half of the model.
(b) The results are reflected about the mirror plane (the yellow rectangle) to create an image of the full model. The mirror plane can be optionally shown or hidden.
Figure 2: Mirror Planes
The model can be mirrored by right-clicking on the appropriate entry in the Mirror Planes branch of the tree view for the current presentation and choosing Activate. To remove the mirror operation, right-click the appropriate plane and clear Activate. To position the mirror plane along the normal direction, right-click and choose Edit Offset. The Offset Distance is the coordinate of the mirror plane, where a positive value is along the positive X, Y, or Z axis normal to the plane. Activating multiple mirror planes will mirror the original model and all the reflections created by other mirrors. For example, a one-eighth symmetry model can be mirrored about the XZ plane to represent a 1/4 symmetry model, which can be mirrored about the YZ plane to represent a 1/2 symmetry model, which can be mirrored about the XY plane to represent the full model. The order of activating the mirror planes is not important.
The transparency of the mirror plane can be adjusted by using Results Options View Settings Transparency Level, or by right-clicking on any mirror plane entry in the tree view and choosing Transparency Level. All mirror planes use the same transparency.
The text that appears in the display area is an annotation. You can modify existing annotations and add additional ones by right-clicking on the Annotations branch (or one the existing annotations) in the tree view for the current presentation. When using Add or Edit, the Annotation dialog appears; the sections are as follows:
Annotation text Type the text to show in the display area. Use the bump-out arrow to enter model-specific information such as the filename, load case number, and so on. Multiple lines can be created either by using the <Enter> key while typing the text, or by adding the new line code (either with the bump-out or by typing \n). The Font button is used to format the entire annotation text (font type, size, color, and so on) using a standard Windows Font dialog. Some letters and characters may be clipped-off when using an italics font depending on the font type.
The Saved Presentations branch of the tree view accesses the default presentations and your saved presentations. Right-click and choose Activate to open the corresponding presentation. Note how this loads the window into the Presentations branch of the tree view.
The Filter Modules branch of the tree view is used to set selection filters. A selection filter is used to make it easier to select results of interest while not selecting other items. For example, to sum the heat flow through all the convection faces, use a filter as follows:
The Contact Diagnostic Probe is used in a nonlinear stress analysis with surface to surface contact to track down areas of contact difficulties. When activated and when a contact problem occurs, the diagnostic probe will appear on the model, and the contact pair is identified in the tree. Two probes per contact pair can appear on the model, one for each diagnostic described below.