allow a collection of elements to be grouped together and all but the
retained degrees of freedom eliminated on the basis of linear response within
the group;
are used in the same manner as any of the standard element types in
the
Abaqus
element library once created as described in
Generating Substructures;
can be used in stress/displacement and in coupled acoustic-structural analyses (however,
frequency-based substructures are supported only in direct steady-state dynamic analyses);
have linear response but allow for large translations and large
rotations;
are particularly useful in cases where identical pieces appear several
times in a structure (such as the teeth of a gear) since a single substructure
can be used repeatedly;
can be translated, rotated with respect to the global system, and
reflected in a plane when they are used;
are connected to the rest of the model by the retained degrees of
freedom at the retained nodes;
might contain a set of internal load cases and boundary conditions that can be activated and
scaled;
can include dynamic effects by including retained eigenmodes; and
appear to the rest of the model as a stiffness, optional mass,
damping, and a set of scalable load vectors.
Substructures are collections of elements from which the internal degrees of freedom have been
eliminated. Retained nodes and degrees of freedom are those that are recognized externally
at the usage level (when the substructure is used in an analysis), and they are defined
during generation of the substructure. Factors that determine how many and which nodes and
degrees of freedom should be retained are discussed below and in Generating Substructures.
A substructure can be considered as a special type of element (and is
sometimes referred to as a superelement). The retained nodes of a substructure
form its connectivity. Multiple instances of a substructure (superelement) can
appear in a model.
Why Use Substructures?
There are a number of good reasons to use substructures.
Computational Advantages
System matrices (stiffness, mass) are small as a result of
substructuring. Subsequent to the creation of the substructure, only the
retained degrees of freedom and the associated reduced stiffness (and mass)
matrix are used in the analysis until it is necessary to recover the solution
internal to the substructure.
Efficiency is improved when the same substructure is used multiple
times. The stiffness calculation and substructure reduction are done only once;
however, the substructure itself can be used many times, resulting in a
significant savings in computational effort.
Substructuring can isolate possible changes outside substructures to
save time during reanalysis. During the design process large portions of the
structure will often remain unchanged; these portions can be isolated in a
substructure to save the computational effort involved in forming the stiffness
of that part of the structure.
In a problem with local nonlinearities, such as a model that includes
interfaces with possible separation or contact, the iterations to resolve these
local nonlinearities can be made on a very much reduced number of degrees of
freedom if the substructure capability is used to condense the model down to
just those degrees of freedom involved in the local nonlinearity.
Organizational Advantages
Substructuring provides a systematic approach to complex analyses. The
design process often begins with independent analyses of naturally occurring
substructures. Therefore, it is efficient to perform the final design analysis
with the use of substructure data obtained during these independent analyses.
Substructures provide a clean and simple way of sharing structural information. In large design
projects large groups of engineers must often conduct analyses using the same
structures.
Many practical structures are so large and complex that a finite
element model of the complete structure places excessive demands on available
computational resources. Such a large linear problem can be solved by building
the model, substructure by substructure, and stacking these level by level
until the whole structure is complete and then recovering the displacements and
stresses locally, as required.
Substructure Size
The retained nodal degrees of freedom and the generalized degrees of freedom associated with the
substructure dynamic modes form a full set of the substructure degrees of freedom. The total
number of substructure degrees of freedom is called the substructure size. Abaqus limits the substructure size to 16,384 for substructures used in Abaqus and to 46,340 for substructures generated in Abaqus and used outside of Abaqus, such as for flexible body dynamics workflows (see Generating a Flexible Body).
Valid Procedures
Substructures can be used without restriction in the following procedures:
Substructuring introduces no additional approximation in linear static
structural analysis: the substructure is an exact representation of the linear,
static behavior of its members. The principal drawback to the use of
substructures in stress/displacement analyses is that a substructure's
stiffness matrix is fully populated (no zero terms) and, therefore, may be very
large if the substructure has a large number of retained degrees of freedom.
This, in turn, may mean that the wavefront of the model within which
substructures are used may be large, thus leading to long computer times to
solve the equations.
This difficulty can often be avoided by choosing the substructure's
boundaries carefully or by reusing several smaller substructures rather than a
single larger substructure. In some cases it is possible to take advantage of
the fact that
Abaqus/Standard
allows individual degrees of freedom to be retained, rather than the whole set
of degrees of freedom at a node. For example, in contact problems without
friction only the displacement component normal to the surface need be retained
for the contact solution. Nodal transformations can be helpful in orienting the
displacement components at surface nodes for this purpose (see
Transformed Coordinate Systems).
In a static analysis involving a substructure containing acoustic elements,
the results will differ from the results obtained in an equivalent static
analysis without substructures. The acoustic-structural coupling is taken into
account in the substructure (leading to hydrostatic contributions of the
acoustic fluid), while the coupling is ignored in a static analysis without
substructures.
Using Substructures in Dynamic Analysis
Substructures introduce approximations in dynamic analysis. The default
approach to the dynamic representation of a substructure is to reduce its mass
and damping matrix with the same transformation as is used for its stiffness
matrix, which is known as “Guyan reduction.” This approach assumes that the
response between the eliminated and retained degrees of freedom is correctly
represented by the static modes only. This representation may not be accurate
if dynamic modes within the substructure are important. The dynamic
representation may be improved for Guyan reduction by retaining additional
physical degrees of freedom that are not required to connect the substructure
to the rest of the model. For example, if the substructure is a plate or a
beam, some transverse displacements (and, perhaps, in-surface rotation
components) might be included as retained degrees of freedom for this purpose.
For more details regarding Guyan reduction, see
Substructuring and substructure analysis.
“Dynamic mode addition” can be used as an alternative to Guyan reduction.
This approach involves adding generalized degrees of freedom associated with
the eigenmodes extracted for the substructure. This improves dynamic behavior,
but it introduces the additional cost of extracting the eigenmodes for the
constrained substructure. For more details regarding dynamic mode addition, see
Substructuring and substructure analysis.
The reduction methods can be applied simultaneously to different
substructures within the same structure. Definition of the reduced mass matrix
is discussed further in
Generating Substructures.
Using Substructures in Geometrically Nonlinear Stress/Displacement Analysis
Substructures may undergo large motions if geometric nonlinearities are
considered in a particular stress/displacement analysis (see
About Static Stress Analysis Procedures).
Abaqus/Standard
will account for the large rigid body rotations and translations of the
substructure. However, the substructure is assumed to undergo small (linear
elastic) deformations at all times during the geometrically nonlinear analysis.
An equivalent rigid body rotation for each substructure is computed during each
equilibrium iteration using the retained nodes of the substructure. The
substructure's mass, damping, stiffness matrix (including the retained
eigenmodes), and force vectors are then rotated appropriately using the
equivalent rigid body rotation. Appropriate (rotated) linear perturbation
displacements (strain-inducing displacements relative to the rotating reference
configuration) are used to compute the internal force associated with the
substructure. Degrees of freedom at a node should not be retained selectively
if the substructure is to be used in geometrically nonlinear analysis. Coupled
acoustic-structural substructures should not be used in geometrically nonlinear
analyses.
Comparison with Component Mode Synthesis
The component mode synthesis method has been developed to permit the
structure to be subdivided into components (substructures), with most of the
analysis being done on the smaller components to develop an approximate model
for the entire structure.
The substructures in
Abaqus/Standard
are, in fact, a particular case of the component mode synthesis method extended
to allow for large rotations and translations of the substructure (component)
in the geometrically nonlinear analysis. The component mode synthesis method is
based on the assumption that the small deformations of a substructure can be
modeled using a collection of modes. The most frequently used modes in the
literature are typically referred to as follows:
constraint modes, which are static shapes obtained by giving each
retained degree of freedom in the substructure a unit displacement while
holding all other retained degrees of freedom fixed;
fixed-interface normal modes, which are obtained by fixing the retained
degrees of freedom and computing the eigenmodes of the substructure;
free-interface normal modes, which are obtained by computing the
eigenmodes of the substructure with free (not fixed) retained degrees of
freedom; and
mixed-interface normal modes, which are obtained by fixing a part of the
retained degrees of freedom and computing the eigenmodes of the substructure.
The constraint modes are precisely the static modes (see
Substructuring and substructure analysis)
used by
Abaqus/Standard.
You include these modes in the substructure's representation by specifying the
degrees of freedom that are to be retained (see
Defining the Retained Nodal Degrees of Freedom).
The fixed-interface, free-interface, or mixed-interface normal modes are the
eigenmodes extracted in the eigenfrequency extraction step at the generation
level, and these modes represent particular cases of substructure dynamic modes
allowed in
Abaqus
(see
Defining the Generalized Degrees of Freedom).
You include the dynamic modes in the substructure's representation by selecting
the eigenmodes to be used.
Including Substructures in a Model
When a substructure is used in a model, it is assigned an element number and
defined by nodes just like any other element.
Use an element definition (Element Definition) with a
substructure identifier to include substructures in the definition of another substructure
(nested substructure) or in an analysis model.
In the element definition you define the substructure's element number at the usage level and
assign node numbers to the substructure's retained nodes. You can define more than one
substructure per element definition.
Once a substructure is introduced by an element definition, it is treated like any other element
in the model, except that its response can be linear only (although it can be used as a part
of a model that includes nonlinear effects, including large displacements).
Using substructures requires that the substructure database be available. All the files
generated for the substructure (including the
name.sim file and, optionally, the
substructure model data file and the
name.prt,
name.stt, and
name.mdl files) must be available if
recovering substructure results is performed in the substructure usage analysis.
Abaqus distinguishes between different substructures by their unique substructure names. The
substructure name is a significant part of the substructure element definition.
Two methods are available for including substructures in a model: use of the generic
substructure element type SUBSTR and use
of the Zn-type identifier. Although Abaqus supports both methods, the method using the generic substructure element type
SUBSTR is preferred over the method
using the Zn-type identification.
Preferred Method for Including Substructures in a Model
The preferred method for including substructures in a model is to associate all elements
with the generic substructure element type
SUBSTR.
If the substructure database files are located in the user directory, you can specify
only the substructure name. If the substructure database files are located outside of the
user directory, you must include the relative path to the file location.
Alternative Method for Including Substructures in a Model
The alternative method for including substructures in a model is to associate all
elements with the Zn type identification. In this method, the
substructure name is formed from a prefix and a Zn-type
identifier (for example,
name_Zn).
Ordering of the Substructure Nodes on the Usage Level
The node numbers that are used when a substructure is created and the node
numbers that are associated with the substructure when it is used are entirely
independent. The ordering of the retained nodes when the substructure is used
can be defined in two different ways:
The nodes can be provided in the same order that they were listed in the
substructure definition. In this case you must prevent the sorting of the
retained nodes when you specify the retained degrees of freedom (see
Preventing the Degrees of Freedom from Being Sorted).
Duplicate nodes are not combined if the retained nodes are not sorted.
Therefore, if the same nodes are specified more than once in the list of
retained degrees of freedom to retain different degrees of freedom, the
corresponding nodes at the usage level must appear the same number of times.
The substructure nodes must be specified in the same order as the
retained nodes sorted into ascending numerical order according to their numbers
used within the substructure. This approach is the default when you specify the
retained degrees of freedom.
In either case you must ensure that the nodes match up properly whenever a
substructure is used.
Interpreting the Model Output in the Data File
Substructures included in the model can have nested substructures; these nested
substructure can also have nested substructures as well, up to 20 levels. All of these
substructures constitute the substructure tree of the model, which is printed to the data
file with the relevant indentation. For each substructure element, the tree shows the
substructure element's label, the full name of the associated substructure, and the suffix
for the recovery output database name.
If model definition data are written to the data file (Controlling the Amount of analysis input file processor Information Written to the Data File), substructure
instances are identified in the data (.dat) file by the substructure
identifier followed by an F and two digits that indicate the substructure database number.
The full name of the substructure database associated with this number is also contained
in the model output.
Defining the Substructure's Properties
You associate a property definition with each substructure in the model. The
property definition serves the following purposes:
It defines any translation, rotation, and reflection of the substructure
at the usage level.
It allows a tolerance to be set to ensure that the coordinates of the
usage level nodes match the coordinates of the nodes used to generate the
substructure.
It controls using various sources of substructure damping in the dynamic
analysis at the usage level.
Translating, Rotating, and Reflecting a Substructure
Translation, rotation, and/or reflection (in that order) of a substructure
can be specified in a substructure property definition.
Specify a translation by giving a translation vector. Specify a rotation by
giving two points, a and b, defining
a rotation axis plus a right-handed angular rotation around that axis. Specify
a reflection by giving three non-colinear points in the reflection plane.
A translation does not affect the substructure's stiffness or mass: the
principal reason to apply a translation is to enable the tolerance check on
nodal coordinates as discussed later. Rotation and/or reflection of a
substructure affect the substructure's stiffness and mass. The substructure
load case definitions are rotated and/or reflected in the same way as the
substructure's stiffness and mass; therefore, all loads within substructure
load cases are applied in the local directions associated with the substructure
when it was created.
For distributed loads (for example, pressure loading of a surface) this
application is precisely what is desired. However, distributed body forces in
coordinate directions (BX, BY, BZ) are applied in the substructure's local directions instead of in
the global directions, which may not be what is needed. Similarly, distributed
loadings that depend on position (for example, hydrostatic pressure or
centrifugal loads) are based on the substructure's local coordinates and not on
the substructure position during usage. Be careful to ensure that loading of a
rotated or shifted substructure is correct for its usage.
Whenever a substructure is translated, rotated, and/or reflected, the
degrees of freedom at any retained nodes are with respect to the coordinate
directions at the usage level. Therefore, if all of the degrees of freedom of a
node are not retained or if a two-dimensional substructure is used in a
three-dimensional model with rotation out of the
x–y plane, additional degrees of
freedom may be activated due to rotation and/or reflection. Be careful to check
the validity of the substructure usage in such cases.
Setting a Tolerance on the Substructure Nodes
One difficulty with using large substructures is ensuring that the retained
nodes in the substructure are connected to the correct nodes on the usage level
(after substructure translation, rotation, and/or reflection, if applicable).
Therefore,
Abaqus/Standard
checks that the coordinates of the retained nodes match the coordinates of the
corresponding nodes on the usage level. A substructure does not require any
coordinates on the usage level because it consists only of a stiffness matrix,
a mass matrix, and a number of load cases. Nevertheless, it is usually a good
check of a model's validity to verify that the substructure and the model into
which it is introduced are geometrically consistent.
To check the coordinates, you can set a tolerance on the distance between
usage level nodes and the corresponding substructure nodes. This tolerance
indicates the largest deviation allowable before a warning is issued. If you do
not specify this tolerance, the default is to use a tolerance of
10−4 times the largest overall dimension within the substructure. If
you specify a tolerance of 0.0, the position of the retained nodes is not
checked.
The geometric check is based on the coordinates of the retained nodes after
translation, rotation, and/or reflection of the substructure at the usage
level; motions of these nodes that occur as a result of geometrically nonlinear
preloading during generation of the substructure are not considered in this
check.
Defining Substructure Damping
Defining substructure damping at the substructure usage level means defining
viscous and structural damping matrices for the finite elements associated with
the substructures.
Abaqus
allows you to choose a particular source of damping for a substructure, to add
several sources, or to exclude the damping effects for a substructure at the
usage level. All options defining the substructure damping belong to a
substructure property definition and affect only the finite elements of the
substructure type associated with the substructure property.
Sources of Substructure Damping
You can choose to model the damping of a substructure at the usage stage
by using the reduced substructure damping matrices computed during the
generation stage and stored on the substructure database. We denote the reduced
viscous damping matrix of a substructure as
and the reduced structural damping matrix of a substructure as
.
Alternatively, you can introduce the stiffness and mass proportional damping
matrices by multiplying the reduced substructure stiffness and mass matrices,
and ,
respectively, with the factors defined within the substructure property
definition at the usage stage. You can also combine both damping sources or
exclude the effects of damping altogether at the usage level. Finally, you can
introduce viscous and structural modal damping matrices for a substructure
specifying damping coefficients for the substructure eigenmodes calculated at
the generation stage and stored on the substructure database.
The substructure modal damping contributes to the damping matrices for the
finite elements associated with a substructure, and it can be used instead of
or together with the other substructure damping sources. To define the
substructure modal damping matrix, you specify the diagonal damping matrix on
the substructure modal subspace. This matrix is transformed to the substructure
degrees of freedom space to be added to the damping matrix of the finite
element associated with the substructure.
Controlling the Sources of Substructure Viscous Damping
In the general case the substructure type element viscous damping matrix
at the usage stage is defined by the following matrix equation:
You can specify substructure viscous damping using substructure damping
controls and/or substructure viscous modal damping. If you specify substructure
viscous modal damping, it is used in combination with all other activated
viscous damping sources to form the viscous damping matrix of the finite
element. Defining the substructure viscous modal damping is discussed in more
detail in
Defining Substructure Viscous Modal Damping
below.
Controlling the Sources of Substructure Structural Damping
In the general case the substructure type element structural damping
matrix is defined by the following equation:
You can specify substructure structural damping using substructure damping
controls and/or substructure structural modal damping. If you specify
substructure structural modal damping, it is used in combination with all other
activated structural damping sources to form the structural damping matrix of
the finite element. Defining the substructure structural modal damping is
discussed in more detail in
Defining Substructure Structural Modal Damping
below.
Defining Substructure Damping Factors
By default, the damping factors,
and ,
and the structural damping factor, ,
used to define stiffness proportional and mass proportional damping for a
substructure are zeros.
Defining Substructure Viscous Modal Damping
Substructure viscous modal damping is defined for the substructure
eigenmodes extracted at the substructure generation level. The mode numbers and
the eigenfrequencies used to define substructure viscous modal damping come
from the solution of the substructure eigenvalue problem at the generation
level.
Defining Substructure Structural Modal Damping
Substructure structural modal damping is defined for the substructure
eigenmodes extracted at the substructure generation level. The mode numbers and
the eigenfrequencies used to define substructure structural modal damping come
from the solution of the substructure eigenvalue problem at the generation
level.
Controlling the Use of Frequency-Based Substructures
Frequency-based substructures are supported only in direct steady-state dynamic analyses
(see Direct-Solution Steady-State Dynamic Analysis). When used at the same frequencies as
those used for generation, frequency-based substructures represent the substructure with
dynamic exactness. This allows for large models to reduce to very small models without any
loss of accuracy. By default, the frequency-based substructure is used only at those
frequencies at which the frequency-based substructure is generated (see Generating Frequency-Based Substructures), and the conventional substructure
is used at all the nonmatching frequencies. Therefore, the dynamic representation of the
substructure is exact at the matching frequencies and is the same as that of the
conventional substructure at nonmatching frequencies. The frequency-based substructure
operators from the
jobname_Zn.sim
file obtained from the substructure generation procedure are used.
You can choose to use the frequency-based substructure at all frequencies of a direct
steady-state dynamic analysis. However, the response at frequencies that do not match
those used at generation is only an approximation. This approximation is based on the
averaging of the frequency-based substructure operators corresponding to neighboring
frequencies. If the frequency of interest is beyond the range of frequencies at which the
frequency-based substructure is generated, this averaging is not possible, and Abaqus issues an error in the jobname.msg
file. You can also disable the use of frequency-based substructures at any frequency, even
if the frequency-based substructure operators are available in the
jobname_Zn.sim
file. In this case the conventional substructure is used instead at all frequencies.
Substructure modal damping is allowed only when the substructure does not contain
frequency-based substructures or the use of frequency-based substructures is disabled;
otherwise, substructure modal damping is ignored. Similarly, substructure loads are
allowed in the direct steady-state dynamic analysis only when the substructure does not
contain frequency-based substructures or the use of frequency-based substructures is
disabled.
Defining Kinematic Constraints and Transformations
All kinematic boundary conditions, MPCs,
and transformations can be applied to retained degrees of freedom at the usage
level. These specifications can be changed from step to step in the usual way.
In this respect substructures and their retained nodes act in an identical
manner to regular elements and their nodes.
Defining Transformations at Retained Nodes
If a nodal transformation (Transformed Coordinate Systems)
is used during substructure generation at a retained node, the transformations
are built into the substructure. This creates an inconsistency when the
substructure node is attached to a standard
Abaqus
element since
Abaqus/Standard
uses the retained degrees of freedom directly without checking their
directions. Therefore, it is suggested that this situation be avoided.
If a nodal transformation must be used, the resulting inconsistency can be
resolved by retaining all degrees of freedom at the node and applying a linear
constraint equation (Linear Constraint Equations)
as follows. At any point where such a transformed substructure node is attached
to a global model, define two coincident nodes on the usage level,
P and Q, for example. Use node
P for the substructure at the usage level (defined with an
element definition); the local directions of the degrees of freedom are already
built in at this node. Use node Q for all standard
Abaqus
elements attached to this point. Use a local transformation at node
Q to transform the degrees of freedom to the same local
directions that are built-in for node P. Now use a linear
constraint equation to equate the individual degrees of freedom at nodes
P and Q.
Performing Parametric Studies on the Substructure Stiffness Matrix
You can change the substructure properties to perform parametric studies by controlling the
amount of unsymmetry in a substructure stiffness matrix. This feature is allowed only in
complex frequency analyses using the unsymmetric solver. You control the unsymmetry by
specifying a factor for the unsymmetric part of the substructure stiffness. This feature
works only when both a symmetric and an unsymmetric instance of the substructure stiffness
matrix are available (see Generating a Reduced Stiffness Matrix for a Substructure).
You specify an element set on which you want to perform parametric studies. Abaqus ignores any elements that are not substructures. You specify the factor of unsymmetry, , in the equation for the stiffness matrix:
where is the stiffness matrix computed by controlling the stiffness unsymmetry
factor, and and are the symmetric and unsymmetric instances, respectively, of the
available substructure stiffness matrix.
The default value of the unsymmetry factor is 1.0. You can perform parametric studies on
different sets of elements, and the effect of the changes in the stiffness matrix is local
to the current step.
Applying Loads to a Substructure
Loads that are to be applied to a substructure within an analysis (at the
usage level) must be specified during the substructure generation step by
defining a substructure load case or by requesting that the substructure's
gravity load vectors be calculated (see
Defining Substructure Load Cases for Subsequent Loading in an Analysis).
A load case can be made up of any combination of loadings, and multiple load
cases can be defined for any given substructure.
When you activate load cases created for a substructure, you specify the
element number or element set name of the substructures, the associated
substructure load case names, and the scaling multipliers for the specified
substructure load case loads. To reproduce the loading conditions defined
during substructure generation exactly, use a magnitude of 1.0.
Boundary conditions specified during a substructure's generation are always
present. They are effectively built into the substructure and cannot be
removed. Boundary conditions cannot be specified within the substructure load
cases. See
Generating Substructures
for further information about defining boundary conditions in substructures.
Modifying or Removing Load Cases
By default, substructure loads are applied as modifications of existing
loads or in addition to any loads previously defined. You can remove all
previously defined loads and, optionally, specify new loads when you activate a
load case. Boundary conditions cannot be removed.
Specifying Time-Dependent Load Cases
The magnitude of substructure loads can be varied with time by referring to
an amplitude definition (Amplitude Curves).
Load Cases in Geometrically Nonlinear Analyses
All substructure loads and boundary conditions are applied in a local system
associated with the substructure. Since this local system rotates with the
substructure when large motions are present, these loads and boundary
conditions will rotate as well. As a consequence, you should be careful when
using substructure loads in geometrically nonlinear analyses to ensure that the
loading is in the appropriate direction at the usage level. This situation is
similar to rotating the substructure via a substructure property definition.
Gravity Loading
A distributed load definition can be used to apply gravity loading to a substructure with a
user-defined magnitude, scaled by an amplitude definition, and acting in a specified
direction. To enable gravity loading for a substructure, you must request the calculation
of the substructure's gravity load vectors during the substructure generation step (see
Gravity Loading). In
this case gravity loading should not be defined as part of a substructure load case.
Obtaining Output of the Solution for All of the Substructure Degrees of Freedom
The retained nodal degrees of freedom and the generalized degrees of
freedom associated with the substructure dynamic modes form the full set of the
substructure's degrees of freedom. You can output the solution at all of the
substructure degrees of freedom. This feature is available only for
Abaqus/Standard
transient dynamic analysis; it is not supported for static and linear dynamic
analyses. For more information, see
Defining the Retained Nodal Degrees of Freedom
and
Defining the Generalized Degrees of Freedom.
Obtaining Output for Selected Substructures
By default, the output is performed for all substructures in the model. You
can output the solution for selected substructures by specifying the element
set that contains all the substructure-type elements where you want to output
the solution.
Obtaining Output in Output4 Format
By default, the substructure solution is stored on
SIM, which is a high-performance database
available in
Abaqus.
The substructure output data are stored in files named
jobname_STEPn_m.sim,
where jobname is the name of the input file or
analysis job, n is the number of the
Abaqus
step that generates the substructure output, and m
is the substructure element label defined in the input file. The substructure
output data written to SIM can later be
converted to one of the conventional text or binary formats as a postprocessing
operation.
You can also output the substructure solution in Output4 text format, which
can be used, for example, by the MSC Nastran
finite element solver from MSC.Software Corporation or by the AVL EXCITE™
flexible body dynamics solver from AVL LIST GmbH. The substructure output data
in the OP4 text format are stored in files named
jobname_STEPn_m.op4,
where jobname is the name of the input file or
analysis job, n is the number of the
Abaqus
step that generates the output, and m is the
substructure element label defined in the input file.
Obtaining Output of Results within a Substructure
You can obtain output within substructures used in static, dynamic, eigenfrequency extraction,
and steady-state and transient modal dynamic analyses. The recovery of output is not
possible for substructures used in response spectrum and random response analyses. Output
within a substructure does not include the displacements, stresses, etc. resulting from the
preload deformation of a substructure.
Output within substructures is available in the data
(.dat) file, in the results (.fil)
file, and in output database (.odb) files. Separate output
database files are created for each substructure using the naming convention
inputfile-name_substructure-number.odb.
If a substructure contains a nested substructure, a file called
inputfile-name_substructure-number_nested-substructure-number.odb
is created containing the output for the nested substructure. The
abaqus substructurecombine execution procedure can
combine model and results data from two substructure output databases into a
single output database. For more information, see
Combining Output from Substructures.
Recovery of the solution within substructures requires that the information for recovering the
data within a substructure be available from the .sim,
.prt, .stt, and .mdl files.
Availability of the model data (.odb or .sim) file
is not required but is strongly recommended.
Output is organized substructure by substructure: you direct Abaqus/Standard to go inside a particular substructure and then request output for that substructure.
Results can be recovered within nested multilevel substructures only if the substructure
databases for all substructures in the chain are available.
Substructure output requests are most easily pictured by thinking of
substructures as “levels” of detailed modeling. At the global (top) level we
have the analysis model (for example, an airplane). Dropping down from this
level to the first substructure level, we have the main components of the model
defined as substructures (wings, stabilizer, fuselage, etc.). Dropping down to
the second substructure level, we have other substructures (flaps, tanks,
floors, etc.), which, in turn, may contain third level substructures (spars,
stringers, etc.), and so on. To obtain output, you move down and back up
through these various levels using substructure paths, similar to the way you
navigate a tree structure for file directories. Each substructure path
definition consists of entering into a substructure at the next level down or
leaving the current substructure and moving up one level in the tree.
At the start of the output requests,
Abaqus/Standard
is at the global model level. You must always enter and leave a substructure
consistently, so that after a set of substructure output requests
Abaqus/Standard
is left at the global model level. You must return to the global level (outside
all substructures) before the end of the step definition.
If you enter and leave in the same substructure path definition, the effect
is to leave the substructure and enter another substructure at the same level.
Entering a Substructure for Output
To enter a particular substructure for output, you identify the substructure
by the element number n chosen for it in the model.
All subsequent output requests are for output within that substructure and must
be given in terms of its internal node and element numbers (the node and
element numbers used when the substructure was created).
Leaving a Substructure after Obtaining Output
After you have obtained output for a substructure, you must return to the
level of the model of which the substructure forms a part, thus indicating the
end of the output requests for variables within that substructure.
Obtaining Output If Substructures Are Nested
You must enter several substructures if substructures are used at multiple
levels and output is required several levels down.
Example: Obtaining Output within Nested Substructures
For example, suppose that a model includes several substructures at two
levels. Printed output of stress components is required in some elements within
two substructures at the second level, as well as printed output of the
displacements at some of the nodes of one of the first-level substructures.
(Recall that “first-level” refers to substructures used directly in the
analysis model; “second-level” substructures are used as components of
first-level substructures.)
The data might be as follows:
SUBSTRUCTURE PATH, ENTER ELEMENT=N
** This option takes us into element number N, which must be a substructure.SUBSTRUCTURE PATH, ENTER ELEMENT=M
** We now drop down into element number M of this substructure.
** M is the element number used for this substructure when N was created.
** M must refer to a substructure.EL PRINT, ELSET=A1
S
** This option requests stress output in element set A1 of this substructure.
** This element set must have been defined during the creation of substructure M.SUBSTRUCTURE PATH, LEAVE
** This option takes us back up into first-level substructure N.SUBSTRUCTURE PATH, ENTER ELEMENT=P
** This option takes us down into element P, which must again be a substructure in element N.EL PRINT, ELSET=A1S
** This option requests the printing of stress output in element set A1. It is possible that
** this is the same set of elements in the same substructure as was used in the request above
** because substructures M and P may both be copies of the same substructure.
** However, the stresses will presumably be different because they represent the same
** component in different locations in the model.SUBSTRUCTURE PATH, LEAVE
** Back to N.SUBSTRUCTURE PATH, LEAVE
** We are now back at the global level.SUBSTRUCTURE PATH, ENTER ELEMENT=R
** Enter element R at the global level: this element is the substructure in which we want
** to print the displacements.NODE PRINT, NSET=FLANGEU
** This option prints the displacements at all nodes in node set
** FLANGEof the substructure.
** Again,FLANGE must have been defined when the substructure was
** created.SUBSTRUCTURE PATH, LEAVE
** Back to the global level.
Interpreting Nodal Variable Output
The nodal displacements within the substructure do not include the
displacements resulting from the preload deformation if it exists.
If a substructure is rotated and/or reflected, nodal variables are output
relative to the global coordinate system of the analysis. In a geometrically
nonlinear analysis, the nodal displacements will include the large motions
associated with the translation and rotation of the substructure in addition to
the small-strain displacements. If a nodal transformation (Transformed Coordinate Systems)
has been used, nodal output will be in either the local or the global
directions, depending on the nodal output request (see
Output to the Data and Results Files).
If a nodal transformation has been used during substructure generation, the
transformed directions are rotated with the substructure.
Interpreting Element Variable Output
Element output variables within a substructure do not include the values of
the variable resulting from the preload deformation if it exists.
Element variables in continuum elements are output relative to the global
coordinate system of the analysis model or in the local (material) coordinate
system if one has been used (Orientations).
Element output for structural elements is always given with respect to the
element coordinate system used during substructure generation. Integration
point coordinates and local material directions (see
Output to the Data and Results Files)
are given with respect to the global coordinate system.
Element quantities associated with nonlinear preload response (plastic
strains, creep strains, etc.) can be output during a substructure recovery.
Since the response in a substructure during its usage is entirely linear, these
quantities, which are part of the base state, do not change from the values
computed during the preload.
If a substructure was reflected, the element connectivities of continuum
elements written to the substructure instance output database are adjusted so
as not to violate the
Abaqus
convention for counterclockwise element numbering.
You cannot directly obtain the element output for the element centroidal
values or the element output at the element nodes when you recover results
within substructures. This output data can be calculated from the
substructure-related data in the output database file using commands in the
Abaqus Scripting Interface.
Interpreting Results Written to the Results File
Results within substructures can be written to the results file.
Substructure path records are inserted in the results file to indicate the
switch into a substructure: all records following such a record belong to the
substructure defined on that record until the next substructure path record
appears in the file.
Requests for output to the results file will cause
Abaqus/Standard
to write the definitions of elements and nodes at the global level and within
all substructures in the model to the file. As with the results records
themselves, these records for nodes and elements within substructures will be
preceded and followed by substructure path records to indicate that they belong
to that substructure.
Node and element numbers within each substructure are local to that
substructure, so that the same node and element numbers may appear in several
substructures and in the global level model. In such a case the substructure
path records must be used to identify the location of a particular node or
element within the model. If you can ensure that node and element numbers are
unique throughout the entire model, including all substructures, the
substructure path records in the results file can be ignored.
Substructure Compatibility
Only the substructure SIM database (.sim)
and the model data (.odb or .sim) files are
backward compatible. If these files were generated from a previous general release or from a
previous maintenance delivery of the same general release, they can be upgraded to the
current release (see SIM Database Utilities and Output Database Upgrade Utility). Other substructure files (including the
.stt, .prt, and .mdl files)
are not compatible between maintenance deliveries of the same general release. These files
are required only if recovering results within substructures is performed in the
substructure usage analysis. When recovering results, you must regenerate your substructures
in the current release.
Input File Template
The following template can be used to generate a
substructure:
HEADING
…
NODE,NSET=N1Data lines to define the nodes.
…
NSET,NSET=N3Data lines to define the node set members.
…
ELEMENT, TYPE=CPE8, ELSET=E1Data lines to define the elements that make up the substructure.
…
ELSET,ELSET=E3Data lines to define the element set members.
…
SOLID SECTION, ELSET=E1, MATERIAL=M1MATERIAL, NAME=M1ELASTIC
30.E6, 0.3
DENSITY
0.0007324
STEPFREQUENCYData line to specify the number of modes ( m). The FREQUENCY optionis required if modes are requested using the SELECT EIGENMODES option.END STEPSTEPSTATIC
…
Options to define a linear or nonlinear static preload.
…
END STEPSTEPSUBSTRUCTURE GENERATE, NAME=MY_SUBSTRUCTURE, OVERWRITE, MASS MATRIX=YES,
VISCOUS DAMPING MATRIX=YES, STRUCTURAL DAMPING MATRIX=YES,
RECOVERY MATRIX=YES, NSET=N3, ELSET=E3RETAINED NODAL DOFSData lines to define the retained degrees of freedom.SELECT EIGENMODES, GENERATE
1, m, 1
SUBSTRUCTURE LOAD CASE, NAME=LOADSCLOADData lines to define concentrated loading.DLOADData lines to define distributed loading.END STEP
The following template can be used to define substructure
instances: