XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''"> Creating Element Properties
Through the Element Properties application, you define element types (such as beam, shell, and so on) and element-related properties for regions of your model, then assign these definitions to geometric or FEM entities. Element type selection is based on the dimensions of the model and your assumptions about the model’s behavior. Additional properties describe attributes such as the thickness of a plate, the spring constant for a spring, an area for a bar element, materials, and so on.
The Element Properties Application Form
Element properties are grouped in sets. Each set has a unique name that you define, and is associated with one analysis code, analysis type and element type (such as MSC Nastran / Structural / Shell), Element properties that vary reference Fields. For example, thickness that varies spatially would be defined using a field (names preceded by f: are field names).
Important: | Element properties are defined with reference to a specific analysis code. Be sure the proper code and type have been selected before proceeding, via the Preferences/Analysis menu. |
To use the Element Properties Application form:
1. Select Properties from the Patran Main form.
The Element Properties application form appears in your viewport.
2. Select an Action, Dimension, and Type combination at the top of the application form.
The bottom portion of the form varies depending on your selections.
Actions
The table below describes the actions you may choose on the Element Properties form.
Action Descriptions |
Create | Inputs analysis code specific finite element property data and associates that data with selected FEM or geometric entities. |
Modify | Makes any modification desired to Existing Property Sets. |
Delete | Removes element property sets from the database. |
Show | Displays tables listing FEM or geometric entities and their associated properties. Creates scalar, vector, and marker plots of selected properties. |
Dimensions and Types
The following table lists the dimensions and element types you may select in preparation for an MSC Nastran structural analysis.
Dimension | Type |
0D (Point Elements) | Mass, Grounded Spring, Grounded Damper |
1D (Line Elements) | Beam, Rod, Spring, Damper, Gap, 1D Mass |
2D (Plane Elements) | Shell, Bending Panel, 2D-Solid, Membrane, Shear Panel |
3D (Volume Elements) | Solid (Standard or P-element) |
Sample Element Properties Form
The Element Properties form prompts you to specify a property set name, define the application region, and set code-specific options.
Exisitng Property Sets | The names of previously defined property sets are listed in this listbox. |
Property Set Name | If you have selected an existing set from the listbox (or from the viewport), its name appears here. |
Options | These Options pop-up menus are analysis code-specific. Refer to the documentation for your analysis code for help in making the desired selections. |
Input Properties | Click to display the Input Properties subform for the element type and options selected. |
Select Members | Enter IDs for the entities that you wish to add or remove from the Application Region. Type the IDs, or use cursor selection tools. The entities can be FEM, ASM, or SGM entities. |
Sample Input Properties Subform
The Input Properties subform prompts you to provide additional required and optional information. Following is a sample Input Properties subform. The property names shown without parentheses are required by the analysis code.
You will receive an error message if you try to complete an element property that is missing a required input. The property names shown in parentheses are optional. You can provide them, if needed, for your analysis conditions.
