User-defined element library

This section provides a reference to the user-defined elements available in Abaqus/Standard and Abaqus/Explicit.

Element types
Nodal coordinates required
Element property definition
Element-based loading
Element output
Node ordering on elements

Element types

Un: n must be a positive integer ( $0 < n < 10000$ ) that will define the element type uniquely in Abaqus/Standard
VUn: n must be a positive integer ( $0 < n < 10000$ ) that will define the element type uniquely in Abaqus/Explicit

Active degrees of freedom

As defined in the user element definition.

Additional solution variables

You can define solution variables associated with nodes that are not connected to other elements. However, in Abaqus/Standard, definition of constraints with Lagrange multipliers in user elements should be avoided because of potential equation solver problems.

In Abaqus/Explicit definition of constraints with Lagrange multipliers is not possible because the stable time increment would decrease to infinitesimally small values.

Nodal coordinates required

None required for linear user elements.

As needed in user subroutines UEL, UELMAT, or VUEL for general user elements. The maximum number of coordinates per node is specified in the user element definition (see Defining the maximum number of coordinates needed at any nodal point). The first coordinate entries at each node should correspond to the standard Abaqus convention (X, Y, Z or r, z for axisymmetric elements).

Element property definition

For a linear user element the properties are the stiffness and mass, defined via user-defined matrices or read from an Abaqus/Standard results file. If necessary, you can specify Rayleigh damping values for linear user elements in the element property definition.

For a general user element defined via user subroutines UEL, UELMAT, or VUEL, you define the number of element properties in the user element definition and provide the numerical values in the element property definition. The definition of these properties depends on your coding in subroutine UEL, UELMAT, or VUEL.

Input File Usage

UEL PROPERTY

Element-based loading

None for linear user elements.

Un: Distributed load or flux whose magnitude is given via distributed load or distributed flux loading definitions (see Distributed loads or Thermal loads) for a general user element. n must be a positive integer that is passed into user subroutines UEL, UELMAT, or VUEL to identify the particular load type.

UnNU: Available in Abaqus/Standard only. Distributed load or flux that is completely defined as equivalent nodal values inside user subroutine UEL or UELMAT for a general user element. n must be a positive integer: $- n$ will be passed into subroutine UEL or UELMAT when such a load is active to identify the load type. The minus sign on n indicates that the load is of type NU.

Element output

For a linear user element there are no stress or strain components since the element only appears as a stiffness and mass.

For a general user element any stress, strain, or other solution-dependent variables within the element must be defined as solution-dependent state variables by your coding within subroutine UEL, UELMAT, or VUEL. In Abaqus/Standard they can be printed or written to the results file using output variable SDV.

Currently element output to the output database is not supported for user-defined elements.

Node ordering on elements

As defined in the user element definition.