Generating Matrices from Nonlinear Procedures

Introduction

A linearized finite element model can be summarized in terms of load vector and left-side matrices that represent mass and stiffness for static analysis or heat capacity and thermal conductivity for uncoupled heat transfer analysis. This mathematical abstraction serves various purposes. For example, you can use these matrices to exchange model data with other users, vendors, or software packages without exchanging mesh or material information. You can also use these matrices in techniques such as model order reduction. This abstraction can also be extended to transient nonlinear problems, which can be treated as a series of piecewise linear models constructed from matrix data at discrete times.

Matrix generation from nonlinear analyses accounts for all current boundary conditions, loads, and material responses in the model. The generated matrices are stored in a SIM document named jobname_STATICn.sim and jobname_THERMn.sim for static and heat transfer analyses, respectively. Here jobname is the name of the input file or analysis job, and n is the number of the Abaqus static or heat transfer step that generates the matrices.

Defining Matrix Types for a Static Analysis

The discretization in space of the static equation (see About procedures and basic equations) is

\int_{V^{0}} β_{N} : τ^{c} d V^{0} = \int_{S} N_{N}^{T} \cdot t d S + \int_{V} N_{N}^{T} \cdot f d V,

where

$β_{N}$: defines the strain variation from the variations of the kinematic variables,
$τ^{c}$: is the Kirchhoff stress,

$N_{N}$: are the finite element interpolation functions,
$t$: is the traction per unit current area,

$f$: is the prescribed force per unit volume,

$V^{0}$: is the reference volume of the domain,

$V$: is the current volume of the domain, and

$S$: is the surface bounding this volume.

The stiffness matrix, $K$ , is defined as

K_{M N} = \int_{V^{0}} β_{M} : H : β_{N} d V^{0} + \int_{V^{0}} τ^{c} : \partial_{N} β_{M} d V^{0} - \int_{S} N_{M}^{T} \cdot Q_{N}^{S} d S - \int_{V} N_{M}^{T} \cdot Q_{N}^{V} d V,

where

H

is defined in terms of the current state, direction of straining, etc. and on the kinematic assumptions used to form the generalized strains. See Mechanical Constitutive Theories for a detailed discussion of forming

H

for the material models available in Abaqus.

Q_{N}^{S}

and

Q_{N}^{V}

depend on the type of load being considered and represent the variation of the load vector with nodal variables on the surface

S

and the volume

V

, respectively.

For special workflows, the mass matrix $M$ (see Implicit dynamic analysis) is defined as

M_{N M} = \int_{V^{0}} ρ^{0} N_{N} \cdot N_{M} {d V}^{0},

where

ρ^{0}

is the reference density.

Defining Matrix Types for an Uncoupled Heat Transfer Analysis

The continuous time description of the spatially discretized heat transfer equation (see Uncoupled heat transfer analysis) is

\begin{matrix} \int_{V} N^{N} ρ \dot{U} d V = ​ & - \int_{V} \frac{\partial N^{N}}{\partial x} \cdot k \cdot \frac{\partial θ}{\partial x} d V \\ + \int_{V} N^{N} r d V + \int_{S_{q}} N^{N} q d S, \end{matrix}

where $θ$ is the temperature field, $N^{N}$ are the finite element interpolation functions, $ρ$ is the material density, $\dot{U}$ is the material time derivative of the internal energy, $k$ is the (possibly anisotropic) conductivity matrix, $r$ is the prescribed heat flux per unit volume, $V$ is the volume of the domain, and $S_{q}$ is the surface on which heat flux per unit area $q$ is either directly prescribed or specified through film and radiation conditions.

The external flux vector $P$ is defined as

P^{N} = \int_{V} N^{N} r d V + \int_{S_{q}} N^{N} q d S .

The internal flux vector $I$ is defined as

I^{N} = - \int_{V} \frac{\partial N^{N}}{\partial x} \cdot k \cdot \frac{\partial θ}{\partial x} d V .

The net flux vector $F$ is defined as the sum of the internal flux vector $I$ and the external flux vector $P$ . The heat capacity matrix $C$ is defined as

C^{N M} = \int_{V} N^{N} ρ \frac{\partial U}{\partial θ} N^{M} d V .

The thermal conductivity matrix $K$ is defined as

K^{N M} = - \frac{\partial}{\partial θ^{M}} [- \int_{V} \frac{\partial N^{N}}{\partial x} \cdot k \cdot \frac{\partial θ}{\partial x} d V + \int_{V} N^{N} r d V + \int_{S_{q}} N^{N} q d S] .

That is, the thermal conductivity matrix is the negated derivative of the net flux vector with respect to the nodal temperature vector $θ$ and, hence, includes the effect of temperature-dependent flux conditions such as film and radiation.

Generating Assembled or Element-by-Element Matrices

Matrices are written to the SIM document in assembled or element-by-element forms.

Input File Usage

Use the following option to write matrices in assembled form:

*OPERATOR OUTPUT, OPERATOR=ASSEMBLED

Use the following option to write matrices in element-by-element form:

*OPERATOR OUTPUT, OPERATOR=ELEMENT BY ELEMENT

Specifying the Matrix Type

You can generate matrices representing the following model features:

Stiffness
Mass
Heat capacity
Thermal conductivity
Loads
Solutions
Free body response

The thermal conductivity matrix has an unsymmetric contribution if the thermal conductivity property is temperature dependent. This term is taken into account only if the unsymmetric solver has been activated in the step definition (see Defining an Analysis).

The load matrix in uncoupled heat transfer analysis contains either the nodal external flux vector or the net flux vector corresponding to the loading defined in the heat transfer step.

Input File Usage

Use the following option to generate the stiffness matrix from a static analysis:

*OPERATOR OUTPUT, STIFFNESS

Use the following option to generate the mass matrix from a static analysis:

*OPERATOR OUTPUT, MASS

Use the following option to generate the load vector from a static analysis:

*OPERATOR OUTPUT, LOAD

Use the following option to generate the free body response matrix from a static analysis:

*OPERATOR OUTPUT, FREE BODY RESPONSE

Use the following option to generate the solution vector from a static analysis:

*OPERATOR OUTPUT, SOLUTION

Use the following option to generate the heat capacity matrix from an uncoupled heat transfer analysis:

*OPERATOR OUTPUT, HEAT CAPACITY

Use the following option to generate the thermal conductivity matrix from an uncoupled heat transfer analysis:

*OPERATOR OUTPUT, THERMAL CONDUCTIVITY

Use the following option to generate the external flux vector from an uncoupled heat transfer analysis:

*OPERATOR OUTPUT, LOAD=EXTERNAL

Use the following option to generate the net flux vector from an uncoupled heat transfer analysis:

*OPERATOR OUTPUT, LOAD=NET

Generating Matrices for a Part of the Model

By default, matrices are generated for all supported element types in the model. You can request that Abaqus/Standard generate matrices for a part of the model defined by an element set.

Input File Usage

*OPERATOR OUTPUT, ELSET=element set name

Specifying the Frequency of Matrix Generation

By default, matrices are generated for every increment in the step in which it is requested. You can request that Abaqus/Standard generate matrices at a specified frequency.

Input File Usage

Use one of the following mutually exclusive options:

*OPERATOR OUTPUT, FREQUENCY=output frequency

*OPERATOR OUTPUT, NUMBER INTERVAL=number of intervals

Initial Conditions

Matrix generation occurs in a general analysis procedure. Therefore, the generated matrices include the effect of initial conditions when applicable.

Boundary Conditions

Prescribed boundary conditions are either imposed or not imposed on the generated matrices and load vectors, based on user-defined requests.

Loads

All types of loads supported in static analysis and uncoupled heat transfer analysis can be used for matrix generation. For more information on applying loads, see About Loads. For uncoupled heat transfer analysis, load types that are functions of temperature (such as film and radiation) contribute additional “load stiffness” terms to the thermal conductivity matrix.

Predefined Fields

All types of predefined fields can be specified for matrix generation. For more information on specifying predefined fields, see Predefined Fields.

Material Options

All types of materials that are available in Abaqus/Standard for static and uncoupled heat transfer analyses can be used for matrix generation.

Elements

All element types are supported in matrix generation for static analysis.

Only continuum diffusive heat transfer elements and thermal contact elements are supported for thermal matrix generation. Thermal matrices are written to the SIM document only for supported elements.

Output

The generated matrices are written to the output SIM document in either element-by-element or assembled form. For efficiency, only nonzero matrix entries are stored in the SIM document. If the matrix is symmetric, only the nonzero entries in the upper triangular portion of the matrix are stored. You can use the matrix assembly utility (Element Matrix Assembly Utility) to assemble element matrices in the SIM document and/or write assembled matrices to text files.

Limitations

Constraints that are implemented using the degree-of-freedom elimination technique (such as tie constraints) are not processed for thermal matrix output. In addition, cavity radiation effects are not considered for thermal matrix output.

Input File Template

The following template can be used to generate matrices for an Abaqus/Standard static analysis:

*HEADING
…
**
*STEP
Options to define a static analysis.
…
*BOUNDARY
Options to define the boundary conditions for the static step.
**
*CLOAD and/or *DLOAD and/or *DSLOAD
Data lines to define loads
**
*OPERATOR OUTPUT, OPERATOR=ASSEMBLED, MASS, STIFFNESS, LOAD,
FREE BODY RESPONSE, SOLUTION, FREQUENCY=1
**
Options to define the output requests for the static step. 
**
*END STEP

The following template can be used to generate matrices for an Abaqus/Standard uncoupled heat transfer analysis:

*HEADING
…
**
*STEP
Options to define an uncoupled heat transfer analysis.
…
*BOUNDARY
Options to define the boundary conditions for the heat transfer step.
**
*CFLUX and/or *DFLUX and/or *DSFLUX
Data lines to define thermal loading
*FILM and/or *SFILM and/or *RADIATE and/or *SRADIATE
Data lines to define convective film and radiation conditions
**
*OPERATOR OUTPUT, OPERATOR=ASSEMBLED, HEAT CAPACITY, THERMAL CONDUCTIVITY, 
LOAD=NET, FREQUENCY=1
**
Options to define the output requests for the heat transfer step. 
**
*END STEP