<!-- source-page: 811 -->

# 10.3.2 GENERATING THERMAL MATRICES

Product: Abaqus/Standard

# References

• “Element matrix assembly utility,” Section 3.2.28   
• \*ELEMENT OPERATOR OUTPUT

# Overview

Thermal matrix generation:

• allows for the mathematical abstraction of model data such as mesh and material information by generating global or element matrices representing the thermal conductivity, heat capacity, and load at specific times;   
• writes matrix data to a binary SIM document that can be further processed by Abaqus; and   
• can be used only as part of an uncoupled heat transfer analysis.

# Introduction

A linearized heat transfer finite element model can be summarized in terms of the thermal load vector and thermal matrices that represent the heat capacity and the thermal conductivity. 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 thermal matrix data at discrete times.

Thermal matrix generation occurs in a heat transfer analysis and accounts for all the current boundary conditions, loads, and material response in the model. The generated matrices are stored in a SIM document named jobnameTHERMn.sim, where jobname is the name of the input file or analysis job and n is the number of the Abaqus heat transfer step that generates the matrices.

# Defining matrix types

The continuous time description of the spatially discretized heat transfer equation (see “Uncoupled heat transfer analysis,” Section 2.11.1 of the Abaqus Theory Guide) is

$$
\begin{array}{l} \int_ {V} N ^ {N} \rho \dot {U} d V = - \int_ {V} \frac {\partial N ^ {N}}{\partial \mathbf {x}} \cdot \mathbf {k} \cdot \frac {\partial \theta}{\partial \mathbf {x}} d V \\ + \int_ {V} N ^ {N} r d V + \int_ {S _ {q}} N ^ {N} q d S, \\ \end{array}
$$

<!-- source-page: 812 -->

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

The external flux vector is defined as

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

The internal flux vector is defined as

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

The net flux vector is defined as the sum of the internal flux vector and the external flux vector . The heat capacity matrix is defined as

$$
C ^ {N M} = \int_ {V} N ^ {N} \rho \frac {\partial U}{\partial \theta} N ^ {M} d V.
$$

The thermal conductivity matrix is defined as

$$
K ^ {N M} = - \frac {\partial}{\partial \theta^ {M}} \left[ - \int_ {V} \frac {\partial N ^ {N}}{\partial \mathbf {x}} \cdot \mathbf {k} \cdot \frac {\partial \theta}{\partial \mathbf {x}} d V + \int_ {V} N ^ {N} r d V + \int_ {S _ {q}} N ^ {N} q d S \right].
$$

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

# Specifying the matrix type

You can generate thermal matrices representing the following model features:

• heat capacity   
• thermal conductivity   
• loads

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,” Section 6.1.2).

The load matrix 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 heat capacity matrix:

$\boldsymbol { * } \mathrm { E L E M E N T ~ O P E R A T O R ~ O U T P U T } , \boldsymbol { \mathrm { D A M P I N G } }$

<!-- source-page: 813 -->

Use the following option to generate the thermal conductivity matrix:

\*ELEMENT OPERATOR OUTPUT, STIFFNESS

Use the following option to generate the external flux vector:

\*ELEMENT OPERATOR OUTPUT, LOAD, LOADTYPE=EXTERNAL

Use the following option to generate the net flux vector:

\*ELEMENT OPERATOR OUTPUT, LOAD, LOADTYPE=NET

# Generating matrices for a part of the model

By default, thermal 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: \*ELEMENT OPERATOR OUTPUT, ELSET=element set name

# Specifying the frequency of matrix generation

By default, thermal 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: \*ELEMENT OPERATOR OUTPUT, FREQUENCY=output frequency

# Generating assembled matrices

By default, thermal matrices are written to the SIM document in element-by-element form. You can write assembled matrices to the SIM document, which is recommended when thermal matrix output is requested for large element sets or at frequent intervals.

Input File Usage: \*ELEMENT OPERATOR OUTPUT, ASSEMBLE

# Initial conditions

Thermal matrix generation occurs in a general analysis procedure. Therefore, the generated matrices include the effect of initial conditions in transient analyses.

# Boundary conditions

Prescribed temperature boundary conditions are not imposed on the generated thermal matrices and load vector.

# Loads

All types of loads supported in an uncoupled heat transfer analysis can be used for thermal matrix generation. For more information on applying loads, see “Applying loads: overview,” Section 34.4.1. Load types that are functions of temperature (such as film and radiation) contribute additional “load stiffness” terms to the thermal conductivity matrix.

<!-- source-page: 814 -->

# Predefined fields

All types of predefined fields can be specified for thermal matrix generation. For more information on specifying predefined fields, see “Predefined fields,” Section 34.6.1.

# Material options

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

# Elements

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,” Section 3.2.28) 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

```txt
*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 
```

<!-- source-page: 815 -->

\*\*

\*ELEMENT OPERATOR OUTPUT, ASSEMBLE, STIFFNESS, DAMPING,LOAD, LOADTYPE=EXTERNAL, FREQUENCY=1

\*\*

Options to define the output requests for the heat transfer step.

\*\*

\*END STEP

<!-- source-page: 816 -->

<!-- source-page: 817 -->

# 10.4 Symmetric model generation, results transfer, and analysis of cyclic symmetry models

• “Symmetric model generation,” Section 10.4.1   
• “Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full threedimensional mesh,” Section 10.4.2   
• “Analysis of models that exhibit cyclic symmetry,” Section 10.4.3

<!-- source-page: 818 -->

<!-- source-page: 819 -->

# 10.4.1 SYMMETRIC MODEL GENERATION

Product: Abaqus/Standard

# Reference

• \*SYMMETRIC MODEL GENERATION

# Overview

A three-dimensional model can be created in Abaqus/Standard by:

• revolving an axisymmetric model about its axis of revolution;   
• revolving a single three-dimensional sector about its axis of symmetry; or   
• combining two parts of a symmetric three-dimensional model, where one of the parts is the original model and the other part is obtained by reflecting the original model through either a symmetry line or a symmetry plane.

Abaqus/Standard also provides for the transfer of the solution obtained in the original analysis onto the new model (see “Transferring results from a symmetric mesh or a partial three-dimensional mesh to a full three-dimensional mesh,” Section 10.4.2).

Only stress/displacement, heat transfer, coupled temperature-displacement, and acoustic elements can be used to generate a new model.

# Model generation

The symmetric model generation capability can be used to create a three-dimensional model by revolving an axisymmetric model about its axis of revolution, by revolving a single three-dimensional sector about its axis of symmetry, or by combining two parts of a symmetric model, where one part is the original model and the other part is the original model reflected through a line or a plane. The original model must have been saved to a restart file. The symmetric model generation capability is not available for models defined in terms of an assembly of part instances. Therefore, an element set name or a node set name containing quotation marks is not supported.

An entire three-dimensional model—including nodes, elements, section definitions, material and orientation definitions, rebar, and contact pair definitions—is generated from the original model. Symmetric model generation from a model with general contact is not allowed. You must redefine most types of kinematic constraints (“Kinematic constraints: overview,” Section 35.1.1). However, surface-based constraints (“Mesh tie constraints,” Section 35.3.1) and embedded element constraints (“Embedded elements,” Section 35.4.1) defined in the original model will be generated automatically in the new three-dimensional model. Changes made to the model as part of the history data—element or contact pair removal/reactivation (“Element and contact pair removal and reactivation,” Section 11.2.1) or changes to friction properties (“Changing friction properties during an Abaqus/Standard analysis” in “Frictional behavior,” Section 37.1.5)—will not be transferred to the new model. Such changes will

<!-- source-page: 820 -->

have to be redefined in the history data of the new model. All element and node sets defined in the original model will be used in the new model. These sets will contain all of the new elements and nodes that originated from the original sets.

Additional nodes, elements, contact surfaces, etc. can also be defined to create parts of the model that were not specified in the original model. You must ensure that the numbering of these nodes and elements does not conflict with those used by the symmetric model generation capability. You can control the node and element numbering in the new model (as described below for each type of revolved model) so that you can define additional parts of the model without the risk of conflicting element and node labels. The smallest node/element number used in defining additional parts of the new model should be greater than the largest node/element number generated by the symmetric model generation capability.

# Eliminating duplicate nodes

Duplicate nodes will be generated in certain situations. Such nodes can be eliminated to ensure that the mesh is connected properly. Duplicate nodes can be generated on the axis of revolution of a revolved model, on the connection planes between sectors of a periodic model, and on the connection plane between the two parts of a reflected model. You can specify the tolerance distance, d, to be used in the search for duplicate nodes. The default distance is 1.0% of the average element dimension. In some cases a tolerance distance that is smaller than the default value needs to be specified if, for example, the distance between two nodes on one of the connection planes in the original sector of a periodic model is smaller than the default tolerance distance. Closely spaced nodes elsewhere in the model, such as between interface surfaces or on parts of the model that are generated with any of the other model definition options, will not be eliminated.

Input File Usage: Use one of the following options to specify the tolerance to be used in the search for duplicate nodes:

\*SYMMETRIC MODEL GENERATION, PERIODIC, TOLERANCE=d   
\*SYMMETRIC MODEL GENERATION, REVOLVE, TOLERANCE=d   
\*SYMMETRIC MODEL GENERATION, REFLECT, TOLERANCE=d

# Writing the new model definition to an external file

You can specify the name of an external file (without an extension) to which the data for the new model definition will be written. The extension .axi will be added to the file name provided. The file can be edited to modify or to extend the model generated by Abaqus/Standard.

Input File Usage: Use one of the following options:

\*SYMMETRIC MODEL GENERATION, PERIODIC, FILE NAME=name   
\*SYMMETRIC MODEL GENERATION, REVOLVE, FILE NAME=name   
\*SYMMETRIC MODEL GENERATION, REFLECT, FILE NAME=name

# Identifying the restart files

The symmetric model generation capability uses the restart (.res), analysis database (.stt and .mdl), and part (.prt) files from the old model to generate the new model. The name of the restart files from the old model must be specified when the new analysis is executed by using the oldjob parameter