The Loads and Boundary Conditions application (Loads/BCs) provides the ability to apply a variety of static and dynamic loads and boundary conditions to finite element models. Loads/BCs may be associated with geometric entities as well as FEM entities. When associated with geometric entities, they can be transferred to finite elements created on the geometry. Loads and boundary conditions are intended to be created in multiple single purpose groups referred to as sets. These sets are grouped into load cases in the Load Cases application. Fields can be used in the definition of loads and boundary conditions. Loads/BCs sets remain in the database unless specifically deleted and thus provide an archival record.

Loads/BC Set: A Loads/BC set is comprised of a collection of data (which may include fields) that are associated with both an analysis type and geometric and/or FEM entities. Typical examples are displacements associated with nodes in a structural analysis, or heat fluxes associated with surfaces in a thermal analysis.

Load Case: A Load Case is a group of Loads/BCs sets that together define a single analysis case. Load Cases are assembled from the entire array of Loads/BCs sets in the Load Cases Application.

Analysis Type: Analysis types currently supported are Structural, Thermal, and Fluid Dynamics (CFD).

Nodal: This refers to the case where loads or boundary conditions are associated with finite element nodes. A typical case is a specified displacement at a node of a structural finite element.

Element Uniform: This refers to the case where the loads or boundary condition is associated with the element itself and is assumed to be uniform over the element face, or element edge. A typical case is an element temperature.

Element Variable: This refers to the case where the loads or boundary condition is associated with an element, but varies in magnitude over the element, element face or element edge. It may thus have different values at the element’s nodes. This leads to the case where nodes that are common to adjacent elements may be multi-valued in the loads or boundary conditions. A typical example is pressure applied over an element.

Target Element Type: Target Elements are elements selected to be actual or eventual recipients of the desired loads or boundary condition. All elements in a set must be of the same type: either 1D, 2D, or 3D. If more than one type is involved, make a separate set for each. Target Element Types are only required for Element Uniform or Element Variable Loads/BCs sets.

Dynamic Loads/BCs Sets: Dynamic loads and boundary conditions sets are those which have a time-dependent component. They must be associated with a time dependent Load Case, which must be the current case when the set is created. Time and spatial dependencies are assumed to be uncoupled. Dynamic sets are comprised of a static spatial component multiplied by a time varying component. Fields must be used to define the time dependency.

Markers: These are the graphic symbols (e.g., arrows, circles) that appear on the screen and provide visual feedback of the location, type, magnitude and direction of the loads or boundary condition. Their display can be turned on or off in the Plot Marker form, or in the Display/Functional Assignment top menu form. See Rules for Creating/Modifying/Applying Loads and Boundary Conditions, 9 for more details.

Type Prefix: As a convenience, each set is given a type prefix that is displayed when sets of different types are listed together. This prefix is the first five letters of the set type followed by an underscore. For example, a set of displacements named “set_1” would appear as “displ_set_1” when displayed with sets of other types.

The Loads/BCs application has the capability of creating, deleting, modifying, and displaying loads and boundary condition sets. Three Analysis Types are supported: Structural, Thermal, and Fluid Dynamics (CFD).

The sets can be either Static or Time Dependent (dynamic). Time dependency is introduced either through the inclusion of a time dependent field multiplier, or through use of initial condition options (e.g., initial displacements).

The loads and boundary condition set types that can be created depend on the analysis selected. The Loads/BCs set types available are a function for the analysis code set in “Analysis Preferences.” For example, if MSC Nastran is the current analysis code selection then only Structural Loads/BC set types will be available. For structural analyses, nine different set types are supported: displacement, force, pressure, temperature, inertial load, initial displacement, initial velocity, velocity and acceleration. For thermal analyses, sets can include temperature (thermal), convection, heat flux, heat source, and initial temperature. Fluid analysis set types are: inflow (incomp), outflow (incomp), solid wall (incomp), symmetry, inflow (comp), outflow (comp), open flow (comp), solid wall (comp), volumetric and total heat load.

Loads and boundary conditions are created and stored in the database as sets. Each set has a unique name and is associated with one analysis type (e.g., structural), one loads and boundary conditions type (e.g., pressure), and one target element type (e.g., 2D), if applicable. All sets are associated with a load case, which by default is the Current Load Case when the set is created.

Sets can be visually displayed on the screen by markers which show the location, type, magnitude, and direction of the applied loads or boundary condition. Only the static portion of a dynamic Loads/BCs set is reflected in the marker display. Sets can also be displayed as tables.

A powerful capability is the display of any set scalar data directly on the model as a fringe plot. For display purposes, data are treated as “results,” with full user control over the spectrum, method, shading, etc. Data display is scalar, but the data can be pressures, vector component magnitudes, and vector resultant magnitudes. Fringe plots can only be displayed on finite elements. Fringes of a dynamic Loads/BCs set may be displayed at user-specified times.

The use of PCL functions in defining loads and boundary conditions is supported through the use of Fields. Use the PCL option in the Fields function to create the desired input data distribution. The field can be used in the Loads/BCs application by simply selecting it from a listbox display.

Loads/BCs can be defined on geometric entities. These are subsequently evaluated on FEM entities associated to that geometry. This is convenient because remeshing the geometry has no effect on the loads and boundary conditions.

The Loads/BCs function provides: