3.1. Element Input

Element Library includes a summary table of element input. The table usually contains information about the following:

3.1.1. Element Name

An element type is identified by a name (eight characters maximum), such as SOLID285, consisting of a group label (SOLID) and a unique, identifying number (285). The element descriptions in Element Library are arranged in order of these identification numbers. The element is selected from the library for use in the analysis by inputting its name on the element type command (ET). See Element Classifications for a list of all available elements.

3.1.2. Nodes

The nodes associated with the element are listed as I, J, K, and so on. Elements are connected to the nodes in the sequence and orientation shown on the input figure for each element type.

Connectivity can be defined by automatic meshing, or can be input directly (E). The node numbers must correspond to the order indicated in the "Nodes" list. The I node is the first node of the element.

The node order determines the element coordinate system orientation for some element types. See Coordinate Systems for a description of the element coordinate system. Internal nodes

The program also uses internal nodes for elements with Lagrangian multiplier in their formulations, such as the mixed u-P formulation of PLANE182, MPC184 and Lagrangian-multiplier-based contact elements, and other elements such as BEAM188, SHELL208 and PIPE288 with quadratic and cubic options.

Internal nodes are generated automatically during the solution phase of an analysis to make more degrees of freedom available for the elements.

Internal nodes are inaccessible and require no input from you or any other action on your part.

3.1.3. Degrees of Freedom

Each element type has a degree-of-freedom set which constitutes the primary nodal unknowns to be determined by the analysis. The set can consist of displacements, rotations, temperatures, pressures, voltages, etc.

Derived results, such as stresses, heat flows, etc., are calculated from these degree-of-freedom results. You do not explicitly define degrees of freedom on the nodes, as they are implied by the element types attached to them. Your choice of element types is therefore of primary concern in any analysis. Internal Degrees of Freedom

In addition to the standard (external) degrees of freedom, some elements or element-formulation options have internal degrees of freedom that are not user-accessible.

The program typically uses internal degrees of freedom to enhance the gradients of the primary unknowns of the elements so that better element behavior can be obtained, but they may also serve other purposes.

Internal degrees of freedom are not shared with nodes of any other elements so that they can be condensed out at the element level during the solution phase of the analysis.

3.1.4. Material Properties

Most element types use various material properties. Typical material properties include Young's modulus (of elasticity), density, coefficient of thermal expansion, and thermal conductivity. Each property is referenced by a label: EX, EY, and EZ for the directional components of Young's modulus, DENS for density, and so on. All material properties can be input as functions of temperature.

Linear Material Properties

Some properties for non-thermal analyses are called linear properties because typical solutions with these properties require only a single iteration.

Nonlinear Material Properties

Properties such as stress-strain data and B-H curves are called nonlinear because an analysis with these properties usually requires an iterative solution.

Material Property Input

Typically, linear material properties are input via the MP family of commands.

Nonlinear material properties are input via the TB family of commands.

The TB family of commands can, however, be used for some linear material properties (such as anisotropic elasticity, material structural damping, piezoelectric matrix, and piezoresistivity).

Some elements require other special data which must be input iin tabular form. Such data are also input via the TB family of commands and are described with the element in Element Library, or in the Material Reference if they apply to a family of elements.

Materials for Explicit Dynamic Analyses

Material models used in explicit dynamic analyses are discussed in Material Models in the ANSYS LS-DYNA User's Guide.

Supported Material Properties for Each Element

See “Material Properties” in the documentation for each element type.

For a list of elements and the material properties supported for each, see Element Support for Material Models.

3.1.5. Special Element Features

The "Special Features" list in the documentation for each element indicates that certain additional capabilities are available for the element. In most cases, the special features make the element nonlinear and therefore require an iterative solution.

Examples of special element features include:

3.1.6. Sections

Sections are generally used to describe the geometry in the missing direction(s) of an idealized model. By idealizing a structure and capturing calculations that are common to many elements, sections may significantly reduce the number of degrees of freedom and lower computational requirements.

Following are common section types:

  • Beam Sections -- A beam cross section defines the geometry of the beam in a plane perpendicular to the element axial direction.

  • Shell Sections -- A shell cross section defines the geometry of the shell in a plane parallel to the shell x-y plane.

  • Reinforcing Sections -- Reinforcing sections allow you to describe the reinforcing fibers collectively within an existing structure rather than model each fiber individually.

  • Axisymmetric Sections -- An axis of symmetry around which a plane of general axisymmetric solid elements is revolved.

Special section types are also available. For example, rather than describing a missing dimension of the model, a contact section corrects the geometry of a meshed circle, sphere, or cylinder.

For a complete list of available section types, see the SECTYPE command.

3.1.7. Real Constants

Data required for the calculation of the element matrices and load vectors, but which cannot be determined by other means, are input as real constants. Typical real constants include hourglass stiffness, contact parameters, stranded coil parameters, and plane thicknesses.

With each element type that supports them, a description of the real constants is given in the "Real Constants" list. The real constant values that you input (R and RMORE) must correspond to the order indicated in the list.

To learn more about how real constants are used within each element type, see the description of each element type in the Mechanical APDL Theory Reference.

3.1.8. Element Loading

Element loads are surface loads, body loads, inertial loads, and ocean loads. Element loads are always associated with a particular element (even if the input is at the nodes). Certain elements may also have flags.

Flags are not actually loads, but are used to indicate that a certain type of calculation is to be performed. For example, when the FSI (fluid-structure interaction) flag is active, a specified face of an acoustic element is treated as an interface between a fluid portion and a structural portion of the model. Similarly, MXWF and MVDI are flags used to trigger magnetic force (Maxwell surface) and Jacobian force (virtual displacement) calculations, respectively, in certain magnetics elements. Details about flags are discussed under the applicable elements in Element Library.

Flags are associated either with a surface (FSI and MXWF) and are applied as surface loads (below), or with an element (MVDI) and are applied as body loads (below). For the FSI and MXWF flags, values have no meaning - these flags are simply turned on by specifying their label on the appropriate command. For the MVDI flag, its value (which can range from zero to one) is specified, along with the label, on the appropriate command. Flags are always step-applied (i.e., the KBC command does not affect them).

The following topics related to element loading are available:

Also see Nodal Loading, which refers to loads defined at the nodes and are not directly related to the elements. Surface Loads

Some element types allow surface loads. Surface loads are typically pressures for structural element types, convections or heat fluxes for thermal element types, and so on.

Table 3.1:  Surface Loads Available in Each Discipline

DisciplineSurface LoadLabel



PRES [1] [2]



Heat Flux

Infinite Surface





Maxwell Surface

Infinite Surface




Maxwell Surface

Surface Charge Density

Infinite Surface







Fluid-Structure Interface





Superelement Load Vector


  1. Not to be confused with the PRES degree of freedom

  2. Buoyancy, wave, current and other ocean loads can be applied to some line and surface element types. For more information, see OCTYPE and related ocean commands. Applying Surface Loads

Surface loads (such as pressures for structural elements and convections for thermal element) are typically input via the SF and SFE commands.

Surface loads may also be input in a nodal format. For example, rather than applying surface loading to an element face, it may be convenient to apply the loading to the face nodes of an element (which are then processed like face input). For more information, see Nodal Loading. Multiple Surface Loads

Some elements allow multiple types of surface loads (as shown with the load labels listed under "Surface Loads" in the input table for each element type). Also, some elements allow multiple loads on a single element face (as indicated with the load numbers after the load labels).

Load numbers are shown on the element figures (within circles) and point in the direction of positive load to the face upon which the load acts. A surface load applied on the edge of a shell element is on a per-unit-length basis, not per-unit area. Surface Load Labels and Keys

Surface loads are designated by a label and a key. The label indicates the type of surface load and the key indicates where on the element the load acts.

The surface load can be defined on element faces via the SFE command by using a key (LKEY), the load label (Lab), and the load value. The SF command can define surface loads by using nodes to identify element faces. The CONV load label requires two values, the film coefficient and the bulk temperature. Tapered Surface Load

A tapered surface load, which allows different values to be defined at the nodes of an element, can be entered via the SFE command. Tapered loads are input in the same order that the face nodes are listed. Body Loads

Some element types allow body loads. Body loads are typically temperatures for structural element types, heat-generation rates for thermal element types, and so on.

Table 3.2:  Body Loads Available in Each Discipline

DisciplineBody LoadLabel




TEMP [1]



Heat Generation Rate




Current Density

Virtual Displacement

TEMP [1]





Charge Density

TEMP [1]



Heat Generation Rate

Force Density



  1. Not to be confused with the TEMP degree of freedom Applying Body loads

Body loads are designated in the "Input Summary" table of each element by a label and a list of load values at various locations within the element.

Body loads are input via the BF or BFE commands. The load values input on the BFE command must correspond to the order indicated in the "Body Load" list.

Body loads can also be applied in a nodal format. For more information, see Nodal Loading. Temperature Body Loads

For some structural elements, the temperature does not contribute to the element load vector but is only used for material property evaluation. For thermal elements using the diagonalized specified heat matrix option in a transient analyses, a spatially varying heat generation rate is averaged over the element. Heat-generation rates are input per-unit-volume unless otherwise noted with the element. The element format is usually in terms of the element nodes but may be in terms of fictitious corner points as described for each element. Corner point numbers are shown on the element figures where applicable. Inertial Loads

Inertial loads (gravity, spinning, etc.), are applicable to all elements with structural degrees of freedom and having mass (that is, elements having mass as an input real constant or having a density (DENS) material property).

Inertia loads are typically entered via the ACEL and OMEGA commands. Initial Stresses

Initial stresses can be set as constant or read in from a file for most current-technology beam, link, plane, solid, and shell element types.

The INISTATE command sets constant initial stress for selected elements and, optionally, only for specified materials. The command also allows you to read in a file specifying the initial stresses. The stresses specified in the input file can be applied to the element centroids or element integration points, and can be applied to the same points for all selected elements or can be applied differently for each element. The stresses can also be a written to an external file.

For more information about the initial state capability, see the INISTATE command, and Initial State in the Mechanical APDL Advanced Analysis Guide. Ocean Loads

Ocean loads can be applied to line and surface element types that support such loads. Ocean loading includes the effects of waves, current, drag, and buoyancy. Loading occurs via the ocean family of commands.

For more information, see Applying Ocean Loads in the Mechanical APDL Basic Analysis Guide.

3.1.9. Nodal Loading

Unlike element loads, nodal loads are defined at the nodes and are not directly related to the elements.

Nodal loads are associated with the degrees of freedom at the node and are typically entered via the D and F commands (such as nodal displacement constraints and nodal force loads).

The nodal or element loading format may be used for an element, with the element loading format taking precedence.

3.1.10. Element Properties and Controls (KEYOPTs)

Elements use KEYOPTs (or key options) to control element behavior, formulation, and output for some beam and shell elements. The KEYOPT is the most important element input and should be selected with care.

Depending on the element type, the KEYOPTs can be used to control stress states, degrees of freedom, element technologies, formulation options, element coordinate systems, printout, results file (.rst) output, loads, temperatures, and so on.

A basic description of each KEYOPT is given with the detailed description of each element type. Because KEYOPTs can be combined, a great deal of flexibility is available for refining the element type to perfectly suit a specific problem.

KEYOPTs are identified by number, such as KEYOPT(1), KEYOPT(2), and so on. Each KEYOPT can be set to a specific value, as follows:

  • Values for the first six KEYOPTs (KEYOPT(1) through KEYOPT(6)) can be input via the ET or KEYOPT command.

  • Values for KEYOPT(7) or greater are input via the KEYOPT command. Element KEYOPT Defaults

The following topics concern element KEYOPT defaults: Consider Automatic Element Selection

Although element KEYOPT defaults can accommodate many problem types, and KEYOPTs can be adjusted as needed, it is often more convenient to allow automatic selection of element technologies via the ETCONTROL command. The command sets element options based on the associated constitutive models of the element type.

For more information, see Automatic Selection of Element Technologies and Formulations. KEYOPT Settings May Vary Between Products

Exercise caution when using the same input for other ANSYS, Inc. products, as some default KEYOPT settings may vary between products. Such cases are indicated in the "Product Restrictions" section of the affected elements. If you intend to use an input file in more than one product, it is a good practice to explicitly input these settings, rather than letting them default; otherwise, element behavior in the other product may differ.

Release 18.2 - © ANSYS, Inc. All rights reserved.