All Loads/BCs sets created are associated with the Current Load Case. This load case will be the one named “Default” unless a different one is specified. The current load case can be changed from within the Loads/BCs application.

The scope of an individual set is limited to a single analysis type (e.g., structural), a single loads or boundary condition definition (e.g., displacement), a single data set, and either FEM or geometry entity types.

Loads/BCs sets can be created, modified, deleted, and displayed. Set modification is completely general in that this action essentially deletes the original set and replaces it with the modified set. The Create option may also be used to modify a set. The only difference is that you will be prompted with a message warning that the set already exists, and asking whether it can be overwritten.

Creating a new set that is a modification of an existing set is accomplished by selecting an existing set, renaming it, and making the desired modifications using the Create action.

In many cases, a Scale Factor may be specified in the Input Data form. All data in the set will be multiplied by this value. The default scale factor is 1.0.

The region of application on the model of the defined set is established using the standard selection tools. If more than one entity can be selected, a select menu will be displayed. The ID of selected items is displayed in the selection region databox.

It is important that the analysis code to be used is selected prior to creating Loads⁄BCs sets.

Fields are created in the separate Fields Application (Ch. 1). Fields must be created before they can be assigned in the Input Data form.

Depending on the specific analysis code and Loads/BCs type, the loads or boundary condition is associated with either the elements themselves or the nodes. If values are associated with elements, they can be either applied uniformly across the element, element face, or element edge (Element Uniform), or vary across the element based on values at associated nodes (Element Variable). The selection between these two options depends on the method used by the analysis code. Determine what is required before attempting to define element loads.

Loads/BCs applied to elements are defined in terms of local coordinate systems as follows: The 1, 2, and 3 directions are defined to be either consistent with the geometric entity C1, C2, and C3 directions or with respect to the element nodal connectivity as shown.

For a rectangular surface, the C1, C2, and C3 directions form a right-handed coordinate system. The top surface is the side in the plus C3 direction.

For elements, connectivity is used to define a coordinate system. If the connectivity is I-J-K-L, the 1-axis corresponds to the I-to-J direction, the 2-axis the I-to-L direction, and the 3-axis normal to the plane defined by 1 and 2 in a right-handed sense. The top surface is on the positive 3-direction side of the element.

Displacements, forces, velocities, and accelerations are positive in the positive directions of the Analysis Coordinate Frame displayed in the Input Data form.

Positive pressures are those that act inward toward the entity. Negative pressures act outward from the entity and represent a surface “suction.”

When loads and boundary conditions are created, they are automatically displayed with markers. Markers may be arrows, circles, squares, etc. Use the Graphics Preferences form to select the marker options. In general, arrows (also referred to as graphical vectors) are used to display quantities which have a direction. All other types of markers are used to display scalar quantities. Arrow markers can have one, two, or three heads. For example, translational displacements, forces, pressures, and translational velocities are displayed as single-headed arrows. Moments and rotations are displayed as double-headed arrows. Rotational accelerations are displayed as triple-headed arrows. Displacement constraint markers may have one-, two-, or three-headed arrows with no tail. For example, if only a translational constraint is specified, a single-headed arrow will be displayed in the appropriate direction. If only a rotational constraint is specified, then a double-headed arrow will be displayed. If both a translational and rotational constraint are specified in the same direction, then a triple-headed arrow will be displayed.

Marker colors can be changed in the Display/Functional Assignment form in the main form. Marker display for each Loads/BCs set type can be selectively turned ON and OFF from this form.

The Loads/BCs application is nondimensional. Input data units are those required by the analysis code selected. Scale factors can be used for conversion if model units differ from code required units (e.g., metric to English).

Set names can be up to 31 characters long and must be unique. Use descriptive names with words separated by underscores. 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. If only displacement sets are listed, the type prefix is omitted.

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, display method, shading, etc. Data display is scalar, of course, but the data to be plotted can be pressures, vector component magnitudes, and vector resultant magnitudes.

The loads and boundary condition set types that can be created depend on the type of analysis being performed. Three different types are currently supported: Structural, Thermal, and Fluid Dynamics (CFD).

For structural analyses, nine different set types are supported: Displacement, Force, Pressure, Temperature, Inertial Load, Initial Displacement, Initial Velocity, Velocity, and Acceleration. Thermal analyses sets can include Temp (Thermal), Convection, Heat Flux, Heat Source, and Initial temperature. Fluid analysis set types include: Inflow (Incomp), Outflow (Incomp), Solid Wall (Incomp), Symmetry, Inflow (Comp), Outflow (Comp), Open Flow (Comp), and Solid Wall (Comp), Volumetric Heat and Total Heat Load.

Each set type can, in turn, have different element associativities, target element types, and required inputs. The tables on the following pages provide maps of all possibilities and options.