<!-- source-page: 191 -->

# JDLTYP

An array containing the integers used to define distributed load types for the element. Loads of type Un are identified by the integer value n in JDLTYP; loads of type UnNU are identified by the negative integer value in JDLTYP. JDLTYP(K1,K2) is the identifier of the K1th distributed load in the K2th load case. For general nonlinear steps K2 is always 1.

# ADLMAG

For general nonlinear steps ADLMAG(K1,1) is the total load magnitude of the K1th distributed load at the end of the current increment for distributed loads of type Un. For distributed loads of type UnNU, the load magnitude is defined in UEL; therefore, the corresponding entries in ADLMAG are zero. For linear perturbation steps ADLMAG(K1,1) contains the total load magnitude of the K1th distributed load of type Un applied in the base state. Base state loading of type UnNU must be dealt with inside UEL. ADLMAG(K1,2), ADLMAG(K1,3), etc. are currently not used.

# DDLMAG

For general nonlinear steps DDLMAG contains the increments in the magnitudes of the distributed loads that are currently active on this element for distributed loads of type Un. DDLMAG(K1,1) is the increment of magnitude of the load for the current time increment. The increment of load magnitude is needed to compute the external work contribution. For distributed loads of type UnNU, the load magnitude is defined in UEL; therefore, the corresponding entries in DDLMAG are zero. For linear perturbation steps DDLMAG(K1,K2) contains the perturbation in the magnitudes of the distributed loads that are currently active on this element for distributed loads of type Un. K1 denotes the K1th perturbation load active on the element. K2 is always 1, except for steady-state dynamics, where K2=1 for real loads and K2=2 for imaginary loads. Perturbation loads of type UnNU must be dealt with inside UEL.

# PREDEF

An array containing the values of predefined field variables, such as temperature in an uncoupled stress/displacement analysis, at the nodes of the element (“Predefined fields,” Section 34.6.1 of the Abaqus Analysis User’s Guide).

The first index of the array, K1, is either 1 or 2, with 1 indicating the value of the field variable at the end of the increment and 2 indicating the increment in the field variable. The second index, K2, indicates the variable: the temperature corresponds to index 1, and the predefined field variables correspond to indices 2 and above. In cases where temperature is not defined, the predefined field variables begin with index 1. The third index, K3, indicates the local node number on the element.

<table><tr><td>PREDEF (K1,1,K3)</td><td>Temperature.</td></tr><tr><td>PREDEF (K1,2,K3)</td><td>First predefined field variable.</td></tr><tr><td>PREDEF (K1,3,K3)</td><td>Second predefined field variable.</td></tr><tr><td>Etc.</td><td>Any other predefined field variable.</td></tr></table>

<!-- source-page: 192 -->

<table><tr><td>PREDEF (K1, K2, K3)</td><td>Total or incremental value of the K2th predefined field variable at the K3th node of the element.</td></tr><tr><td>PREDEF (1, K2, K3)</td><td>Values of the variables at the end of the current increment.</td></tr><tr><td>PREDEF (2, K2, K3)</td><td>Incremental values corresponding to the current time increment.</td></tr></table>

# PARAMS

An array containing the parameters associated with the solution procedure. The entries in this array depend on the solution procedure currently being used when UEL is called, as indicated by the entries in the LFLAGS array (see below).

For implicit dynamics (LFLAGS(1) = 11 or 12) PARAMS contains the integration operator values, as:

<table><tr><td>PARAMS (1)</td><td> $\alpha$ </td></tr><tr><td>PARAMS (2)</td><td> $\beta$ </td></tr><tr><td>PARAMS (3)</td><td> $\gamma$ </td></tr></table>

# LFLAGS

An array containing the flags that define the current solution procedure and requirements for element calculations. Detailed requirements for the various Abaqus/Standard procedures are defined earlier in this section.

<table><tr><td>LFLAGS (1)</td><td>Defines the procedure type. See “Results file output format,” Section 5.1.2 of the Abaqus Analysis User’s Guide, for the key used for each procedure.</td></tr><tr><td>LFLAGS (2) =0</td><td>Small-displacement analysis.</td></tr><tr><td>LFLAGS (2) =1</td><td>Large-displacement analysis (nonlinear geometric effects included in the step; see “General and linear perturbation procedures,” Section 6.1.3 of the Abaqus Analysis User’s Guide).</td></tr><tr><td>LFLAGS (3) =1</td><td>Normal implicit time incrementation procedure. User subroutine UEL must define the residual vector in RHS and the Jacobian matrix in AMATRX.</td></tr><tr><td>LFLAGS (3) =2</td><td>Define the current stiffness matrix (AMATRX =  $K^{NM} = -\partial F^{N}/\partial u^{M}$  or  $-\partial G^{N}/\partial u^{M}$ ) only.</td></tr><tr><td>LFLAGS (3) =3</td><td>Define the current damping matrix (AMATRX =  $C^{NM} = -\partial F^{N}/\partial \dot{u}^{M}$  or  $-\partial G^{N}/\partial \dot{u}^{M}$ ) only.</td></tr></table>

<!-- source-page: 193 -->

<table><tr><td>LFLAGS (3) =4</td><td>Define the current mass matrix ( $\mathbf{AMATRX} = M^{NM} = -\partial F^{N} / \partial \ddot{u}^{M}$ ) only. Abaqus/Standard always requests an initial mass matrix at the start of the analysis.</td></tr><tr><td>LFLAGS (3) =5</td><td>Define the current residual or load vector ( $\mathbf{RHS} = F^{N}$ ) only.</td></tr><tr><td>LFLAGS (3) =6</td><td>Define the current mass matrix and the residual vector for the initial acceleration calculation (or the calculation of accelerations after impact).</td></tr><tr><td>LFLAGS (3) =100</td><td>Define perturbation quantities for output.</td></tr><tr><td>LFLAGS (4) =0</td><td>The step is a general step.</td></tr><tr><td>LFLAGS (4) =1</td><td>The step is a linear perturbation step.</td></tr><tr><td>LFLAGS (5) =0</td><td>The current approximations to  $u^{M}$ , etc. were based on Newton corrections.</td></tr><tr><td>LFLAGS (5) =1</td><td>The current approximations were found by extrapolation from the previous increment.</td></tr></table>

# TIME(1)

Current value of step time or frequency.

# TIME(2)

Current value of total time.

# Scalar parameters:

# DTIME

Time increment.

# PERIOD

Time period of the current step.

# NDOFEL

Number of degrees of freedom in the element.

# MLVARX

Dimensioning parameter used when several displacement or right-hand-side vectors are used.

# NRHS

Number of load vectors. NRHS is 1 in most nonlinear problems: it is 2 for the modified Riks static procedure (“Static stress analysis,” Section 6.2.2 of the Abaqus Analysis User’s Guide), and it is greater than 1 in some linear analysis procedures and during substructure generation.

<!-- source-page: 194 -->

# NSVARS

User-defined number of solution-dependent state variables associated with the element (“Defining the number of solution-dependent variables that must be stored within the element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide).

# NPROPS

User-defined number of real property values associated with the element (“Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide).

# NJPROP

User-defined number of integer property values associated with the element (“Defining the element properties” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide).

# MCRD

MCRD is defined as the maximum of the user-defined maximum number of coordinates needed at any node point (“Defining the maximum number of coordinates needed at any nodal point” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide) and the value of the largest active degree of freedom of the user element that is less than or equal to 3. For example, if you specify that the maximum number of coordinates is 1 and the active degrees of freedom of the user element are 2, 3, and 6, MCRD will be 3. If you specify that the maximum number of coordinates is 2 and the active degrees of freedom of the user element are 11 and 12, MCRD will be 2.

# NNODE

User-defined number of nodes on the element (“Defining the number of nodes associated with the element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide).

# JTYPE

Integer defining the element type. This is the user-defined integer value n in element type Un (“Assigning an element type key to a user-defined element” in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide).

# KSTEP

Current step number.

# KINC

Current increment number.

# JELEM

User-assigned element number.

# NDLOAD

Identification number of the distributed load or flux currently active on this element.

# MDLOAD

Total number of distributed loads and/or fluxes defined on this element.

<!-- source-page: 195 -->

# NPREDF

Number of predefined field variables, including temperature. For user elements Abaqus/Standard uses one value for each field variable per node.

# UEL conventions

The solution variables (displacement, velocity, etc.) are arranged on a node/degree of freedom basis. The degrees of freedom of the first node are first, followed by the degrees of freedom of the second node, etc.

# Usage with general nonlinear procedures

The values of $u ^ { N }$ (and, in direct-integration dynamic steps, $\dot { u } ^ { N }$ and $\ddot { u } ^ { N } )$ enter user subroutine UEL as their latest approximations at the end of the time increment; that is, at time $t + \Delta t$ .

The values of $H ^ { \alpha }$ enter the subroutine as their values at the beginning of the time increment; that is, at time t. It is your responsibility to define suitable time integration schemes to update $H ^ { \alpha }$ . To ensure accurate, stable integration of internal state variables, you can control the time incrementation via PNEWDT.

The values of $\cdot _ { p ^ { \beta } }$ enter the subroutine as the values of the total load magnitude for the th distributed load at the end of the increment. Increments in the load magnitudes are also available.

In the following descriptions of the user element’s requirements, it will be assumed that LFLAGS(3)=1 unless otherwise stated.

# Static analysis (LFLAGS(1)=1,2)

• $F ^ { N } = F ^ { N } ( u ^ { M } , H ^ { \alpha } , p ^ { \beta } , t )$ .   
• Automatic convergence checks are applied to the force residuals corresponding to degrees of freedom 1–7.   
• You must define AMATRX $= K ^ { N M } = - \partial F ^ { N } / \partial u ^ { M }$ and $\mathbf { R H S } = F ^ { N }$ and update the state variables, $H ^ { \alpha }$ .

# Modified Riks static analysis (LFLAGS(1)=1) and (NRHS=2)

• $F ^ { N } = F ^ { N } ( u ^ { M } , H ^ { \alpha } , p ^ { \beta } )$ , where $p ^ { \beta } = p _ { 0 } ^ { \beta } + \lambda q ^ { \beta } , p _ { 0 } ^ { \beta }$ and $q ^ { \beta }$ are fixed load parameters, and is the Riks (scalar) load parameter.   
• Automatic convergence checks are applied to the force residuals corresponding to degrees of freedom 1–7.   
• You must define $\begin{array} { l l l } { { \tt A M A T R X } } & { = } & { K ^ { N M } } & { = } & { - \partial F ^ { N } / \partial u ^ { M } } \end{array}$ , RHS $\mathbf { \Psi } ( \mathbf { 1 } ) \ = \ \mathbf { \Psi } F ^ { N }$ , and RHS(2) $= \Delta \lambda ( \partial { \cal F } ^ { N } / \partial \lambda )$ and update the state variables, $H ^ { \alpha }$ . RHS(2) is the incremental load vector.

# Direct-integration dynamic analysis (LFLAGS(1)=11, 12)

• Automatic convergence checks are applied to the force residuals corresponding to degrees of freedom 1–7.

<!-- source-page: 196 -->

• LFLAGS(3)=1: Normal time increment. Either the Hilber-Hughes-Taylor or the backward Euler time integration scheme will be used. With set to zero for the backward Euler, both schemes imply

$$
F ^ {N} = - M ^ {N M} \ddot {u} _ {t + \Delta t} + (1 + \alpha) G _ {t + \Delta t} ^ {N} - \alpha G _ {t} ^ {N},
$$

where $M ^ { N M } = M ^ { N M } ( u ^ { M } , \dot { u } ^ { M } , H ^ { \alpha } , p ^ { \beta } , t , . . . )$ and $G ^ { N } = G ^ { N } ( u ^ { M } , \dot { u } ^ { M } , H ^ { \alpha } , p ^ { \beta } , t , . . . )$ ; that is, the highest time derivative of $u ^ { M }$ in $M ^ { N M }$ and $G ^ { N }$ is $\dot { u } ^ { M }$ , so that

$$
- \frac {\partial F ^ {N}}{\partial \ddot {u} ^ {M} {} _ {t + \Delta t}} = M ^ {N M}.
$$

Therefore, you must store $G _ { t } ^ { N }$ as an internal state vector. If half-increment residual calculations are required, you must also store $G _ { t ^ { - } } ^ { N }$ as an internal state vector, where indicates the time at the beginning of the previous increment. For $\alpha = 0 , F ^ { N } = - M ^ { N M } \ddot { u } _ { t + \Delta t } + G ^ { N } { } _ { t + \Delta t }$ and $G _ { t } ^ { N }$ is not needed. You must define $\mathtt { A M A T R X } = M ^ { N M } \left( d \ddot { u } / d u \right) + \left( 1 + \alpha \right) C ^ { N M } \left( d \dot { u } / d u \right) + \left( 1 + \alpha \right) K ^ { N M }$ where $C ^ { N M } = - \partial G ^ { N } { } _ { t + \Delta t } / \partial \dot { u } ^ { M }$ and $K ^ { N M } = - \partial G ^ { N } { } _ { t + \Delta t } / \partial u ^ { M }$ . $\mathbf { R H S } = \mathbf { \nabla } F ^ { N }$ must also be defined and the state variables, $H ^ { \alpha }$ , updated. Although the value of given in the dynamic step definition is passed into UEL, the value of can vary from element to element. For example, can be set to zero for some elements in the model where numerical dissipation is not desired.

• LFLAGS(3)=5: Half-increment residual $( F _ { 1 / 2 } ^ { N } )$ calculation. Abaqus/Standard will adjust the time increment so that $| F _ { 1 / 2 } ^ { N } | ~ < ~ t o l e r a n c e$ (where is specified in the dynamic step definition). The half-increment residual is defined as

$$
F _ {1 / 2} ^ {N} = - M ^ {N M} \ddot {u} _ {t + \Delta t / 2} + (1 + \alpha) G _ {t + \Delta t / 2} ^ {N} - \frac {\alpha}{2} (G _ {t} ^ {N} + G _ {t -} ^ {N}),
$$

where $t ^ { - }$ indicates the time at the beginning of the previous increment ( is a parameter of the Hilber-Hughes-Taylor time integration operator and will be set to zero if the backward Euler time integration operator is used). You must define $\mathbf { R H S } = F _ { 1 / 2 } ^ { N }$ . To evaluate $M ^ { N M }$ and ${ G ^ { N } } _ { t + \Delta t / 2 } , \mathrm { y o u }$ must calculate ${ H ^ { \alpha } } _ { t + \Delta t / 2 }$ . These half-increment values will not be saved. DTIME will still contain $\Delta t \left( { \mathrm { n o t } } \Delta t / 2 \right)$ . The values contained in U, V, A, and DU are half-increment values.

• LFLAGS(3)=4: Velocity jump calculation. Abaqus/Standard solves $- M ^ { N M } \Delta \dot { u } ^ { M } = 0 \mathrm { f o r } \Delta \dot { u } ^ { M }$ , so you must define AMATRX . $\tt A M A T R X = M ^ { N M }$   
• LFLAGS(3)=6: Initial acceleration calculation. Abaqus/Standard solves $- M ^ { N M } \ddot { u } ^ { M } + G ^ { N } = 0$ for $\ddot { u } ^ { M }$ , so you must define $\mathtt { A M A T R X } = M ^ { N M }$ and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = G ^ { N }$ .

# Subspace-based dynamic analysis (LFLAGS(1)=13)

• The requirements are identical to those of static analysis, except that the Jacobian (stiffness), AMATRX, is not needed. No convergence checks are performed in this case.

# Quasi-static analysis (LFLAGS(1)=21)

• The requirements are identical to those of static analysis.

<!-- source-page: 197 -->

# Steady-state heat transfer analysis (LFLAGS(1)=31)

• The requirements are identical to those of static analysis, except that the automatic convergence checks are applied to the heat flux residuals corresponding to degrees of freedom 11, 12, …

# Transient heat transfer analysis $\left( \phantom { - } \theta _ { m a x } \right) \left( \tt L F L A G S \left( 1 \right) = 3 2 , \phantom { - } 3 3 \right)$

• Automatic convergence checks are applied to the heat flux residuals corresponding to degrees of freedom 11, 12, …   
• The backward difference scheme is always used for time integration; that is, Abaqus/Standard assumes that $\dot { u } _ { t + \Delta t } = \Delta u / \Delta t .$ , where $\Delta u = u _ { t + \Delta t } - u _ { t }$ and so $d \dot { u } / d u = 1 / \Delta t$ always. For degrees of freedom 11, 12, …, $\lvert \Delta u \rvert$ will be compared against the user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ , for controlling the time integration accuracy.   
• You need to define $\mathtt { A M A T R X } = K ^ { N M } + ( 1 / \Delta t ) \ C ^ { N M }$ , where $C ^ { N M }$ is the heat capacity matrix and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = F ^ { N }$ , and must update the state variables, $H ^ { \alpha }$ .

# Geostatic analysis (LFLAGS(1)=61)

• Identical to static analysis, except that the automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–8.

# Steady-state coupled pore fluid diffusion/stress analysis (LFLAGS(1)=62, 63)

• Identical to static analysis, except that the automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–8.

# Transient coupled pore fluid diffusion/stress (consolidation) analysis $( ~ { u } _ { w } ^ { m a x } )$ (LFLAGS(1)=64, 65)

• Automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–8.   
• The backward difference scheme is used for time integration; that is, $\dot { u } _ { t + \Delta t } ^ { M } = \Delta u ^ { M } / \Delta t$ , where $\Delta u ^ { M } = u _ { t + \Delta t } ^ { M } - u _ { t } ^ { M }$ .   
• For degree of freedom 8, $| \Delta u ^ { M } |$ will be compared against the user-prescribed maximum wetting liquid pore pressure change, $\Delta u _ { w } ^ { m a x }$ , for automatic control of the time integration accuracy.   
• You must define $\mathtt { A M A T R X } = K ^ { N M } + ( 1 / \Delta t ) \ C ^ { N M }$ , where $C ^ { N M }$ is the pore fluid capacity matrix and $\mathbf { R H S } = F ^ { N }$ , and must update the state variables, $H ^ { \alpha }$ .

# Steady-state fully coupled thermal-stress analysis (LFLAGS(1)=71)

• Identical to static analysis, except that the automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–7 and 11, 12, …

<!-- source-page: 198 -->

Transient fully coupled thermal-stress analysis $( \theta _ { m a x } )$ (LFLAGS(1)=72,73)

• Automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–7 and 11, 12, …   
• The backward difference scheme is used for time integration; that is, $\dot { u } _ { t + \Delta t } ^ { M } = \Delta u ^ { M } / \Delta t .$ where $\Delta u ^ { M } = u _ { t + \Delta t } ^ { M } - u _ { t } ^ { M }$ .   
• For degrees of freedom 11, 12, …, $| \Delta u ^ { M } |$ will be compared against the user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ , for automatic control of the time integration accuracy.   
• You must define $\mathtt { A M A T R X } = K ^ { N M } + ( 1 / \Delta t ) \ C ^ { N M }$ , where $C ^ { N M }$ is the heat capacity matrix and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = F ^ { N }$ , and must update the state variables, $H ^ { \alpha }$ .

# Steady-state coupled thermal-electrical analysis (LFLAGS(1)=75)

• The requirements are identical to those of static analysis, except that the automatic convergence checks are applied to the current density residuals corresponding to degree of freedom 9, in addition to the heat flux residuals.

Transient coupled thermal-electrical analysis $\left( \phantom { - } \theta _ { m a x } \right) \left( \tt L F L A G S \left( 1 \right) = 7 6 , \eta 7 7 \right)$

• Automatic convergence checks are applied to the current density residuals corresponding to degree of freedom 9 and to the heat flux residuals corresponding to degree of freedom 11.   
• The backward difference scheme is always used for time integration; that is, Abaqus/Standard assumes that $\dot { u } _ { t + \Delta t } = \Delta u / \Delta t .$ , where $\Delta u = u _ { t + \Delta t } - u _ { t }$ . Therefore, $d \dot { u } / d u = 1 / \Delta t$ always. For degree of freedom 11 $| \Delta u |$ will be compared against the user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ , for controlling the time integration accuracy.   
• You must define $\mathtt { A M A T R X } = K ^ { N M } + ( 1 / \Delta t ) \ C ^ { N M }$ , where $C ^ { N M }$ is the heat capacity matrix and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = F ^ { N }$ , and must update the state variables, $H ^ { \alpha }$ .

Steady-state coupled thermal-electrical-structural analysis (LFLAGS(1)=102)

• Identical to static analysis, except that the automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–7, 9, and 11.

Transient coupled thermal-electrical-structural analysis $( \theta _ { m a x } )$ (LFLAGS(1)=103,104)

• Automatic convergence checks are applied to the residuals corresponding to degrees of freedom 1–7, 9, and 11.   
• The backward difference scheme is always used for time integration; that is, Abaqus/Standard assumes that $\dot { u } _ { t + \Delta t } = \Delta u / \Delta t .$ , where $\Delta u = u _ { t + \Delta t } - u _ { t }$ . Therefore, $d \dot { u } / d u = 1 / \Delta t$ always. For degree of freedom 11 $| \Delta u |$ will be compared against the user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ , for controlling the time integration accuracy.   
• You must define $\mathtt { A M A T R X } = K ^ { N M } + ( 1 / \Delta t ) \ C ^ { N M }$ , where $C ^ { N M }$ is the heat capacity matrix and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = F ^ { N }$ ; and you must update the state variables, $H ^ { \alpha }$ .

<!-- source-page: 199 -->

“General and linear perturbation procedures,” Section 6.1.3 of the Abaqus Analysis User’s Guide, describes the linear perturbation capabilities in Abaqus/Standard. Here, base state values of variables will be denoted by $u ^ { M } , H ^ { \alpha }$ , etc. Perturbation values will be denoted by $\tilde { u } ^ { M } , \tilde { H } ^ { \alpha }$ , etc.

Abaqus/Standard will not call user subroutine UEL for the eigenvalue buckling prediction procedure.

For response spectrum, random response, transient modal dynamic, and mode-based steady-state dynamic procedures, user subroutine UEL is called only in a prior natural frequency extraction analysis, and the mass and stiffness contributions are taken into account during modal superposition.

For direct-solution and mode-based steady-state dynamic, complex eigenvalue extraction, matrix generation, and substructure generation procedures, Abaqus/Standard will call user subroutine UEL, but only mass and stiffness contributions will be taken into account. The damping contributions will be neglected.

# Static analysis (LFLAGS(1)=1, 2)

• Abaqus/Standard will solve $K ^ { N M } \tilde { u } ^ { M } = \tilde { P } ^ { N }$ for $\tilde { u } ^ { M }$ , where $K ^ { N M }$ is the base state stiffness matrix and the perturbation load vector, $\tilde { P } ^ { N }$ , is a linear function of the perturbation loads, $\tilde { p } ;$ that is, $\tilde { P } ^ { N } =$ $\left( { \partial F } / { \partial \tilde { p } } \right) \tilde { p } .$ .   
• $\mathtt { L F L A G S } \left( 3 \right) = 1$ : You must define $\mathbf { A M A T R X } = K ^ { N M }$ and $\mathbf { R } \mathbf { \bar { H } } \mathbf { S } = \mathbf { \tilde { \Lambda } } \tilde { P } ^ { N }$ .   
• $\mathtt { L F L A G S } \left( 3 \right) = 1 0 0 $ : You must compute perturbations of the internal variables, $\tilde { H } ^ { \alpha }$ , and define RHS $= \tilde { P } ^ { N } - K ^ { N M } \tilde { u } ^ { M } $ for output purposes.

# Eigenfrequency extraction analysis (LFLAGS(1)=41)

$\bullet F ^ { N } = - M ^ { N M } \ddot { \tilde { u } } + G ^ { N } ( u ^ { M } + \tilde { u } ^ { M } , \ldots ) = - M ^ { N M } \ddot { \tilde { u } } + \left( \partial G ^ { N } / \partial u ^ { M } \right) \tilde { u } ^ { M } .$   
• Abaqus/Standard will solve $\begin{array} { r l r } { K ^ { N M } \phi _ { i } ^ { M } } & { { } = } & { \omega _ { i } ^ { 2 } M ^ { N M } \phi _ { i } ^ { M } } \end{array}$ for $\phi _ { i } ^ { N }$ and $\omega _ { i }$ , where $\begin{array} { r l } { K ^ { N M } } & { { } = } \end{array}$ $- \partial F ^ { N } / \partial u ^ { M }$ is the base state stiffness matrix and $M ^ { N M } = - \partial F ^ { N M } / \partial \ddot { u } ^ { M }$ is the base state mass matrix.   
• LFLAGS(3)=2: Define $\mathbf { A M A T R X } = K ^ { N M }$ .   
• LFLAGS(3)=4: Define $\mathtt { A M A T R X } = M ^ { N M }$ .

# Example: Structural and heat transfer user element

Both a structural and a heat transfer user element have been created to demonstrate the usage of subroutine UEL. These user-defined elements are applied in a number of analyses. The following excerpt is from the verification problem that invokes the structural user element in an implicit dynamics procedure:

```python
*USER ELEMENT, NODES=2, TYPE=U1, PROPERTIES=4, COORDINATES=3, VARIABLES=12
1, 2, 3
*ELEMENT, TYPE=U1
101, 101, 102 
```

<!-- source-page: 200 -->

```csv
*ELGEN, ELSET=UTRUSS
101, 5
*UEL PROPERTY, ELSET=UTRUSS
0.002, 2.1E11, 0.3, 7200.
```

The user element consists of two nodes that are assumed to lie parallel to the x-axis. The element behaves like a linear truss element. The supplied element properties are the cross-sectional area, Young’s modulus, Poisson’s ratio, and density, respectively.

The next excerpt shows the listing of the subroutine. The user subroutine has been coded for use in a perturbation static analysis; general static analysis, including Riks analysis with load incrementation defined by the subroutine; eigenfrequency extraction analysis; and direct-integration dynamic analysis. The names of the verification input files associated with the subroutine and these procedures can be found in “UEL,” Section 4.1.14 of the Abaqus Verification Guide. The subroutine performs all calculations required for the relevant procedures as described earlier in this section. The flags passed in through the LFLAGS array are used to associate particular calculations with solution procedures.

During a modified Riks analysis all force loads must be passed into UEL by means of distributed load definitions such that they are available for the definition of incremental load vectors; the load keys Un and UnNU must be used properly, as discussed in “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User’s Guide. The coding in subroutine UEL must distribute the loads into consistent equivalent nodal forces and account for them in the calculation of the RHS and ENERGY arrays.

```csv
SUBROUTINE UEL(RHS,AMATRX,SVARS,ENERGY,NDOFEL,NRHS,NSVARS,
1 PROPS,NPROPS,COORDS,MCRD,NNODE,U,DU,V,A,JTYPE,TIME,
2 DTIME,KSTEP,KINC,JELEM,PARAMS,NDLOAD,JDLTYP,ADLMAG,
3 PREDEF,NPREDF,LFLAGS,MLVARX,DDLMAG,MDLOAD,PNEWDT,
4 JPROPS,NJPROP,PERIOD)
C
INCLUDE 'ABA_PARAM.INC'
PARAMETER ( ZERO = 0.D0, HALF = 0.5D0, ONE = 1.D0 )
C
DIMENSION RHS(MLVARX, * ),AMATRX(NDOFEL,NDOFEL),
1 SVARS(NSVARS),ENERGY(8),PROPS(*),COORDS(MCRD,NNODE),
2 U(NDOFEL),DU(MLVARX, * ),V(NDOFEL),A(NDOFEL),TIME(2),
3 PARAMS(3),JDLTYP(MDLOAD, * ),ADLMAG(MDLOAD, * ),
4 DDLMAG(MDLOAD, * ),PREDEF(2,NPREDF,NNODE),LFLAGS(*),
5 JPROPS(*)
DIMENSION SRESID(6)
C
C UEL SUBROUTINE FOR A HORIZONTAL TRUSS ELEMENT
C
C SRESID - stores the static residual at time t+dt
C SVARS - In 1-6, contains the static residual at time t
C upon entering the routine. SRESID is copied to 
```
