Structural Analysis
Steps
An analysis case is a template (a set of objects sets)
for defining environmental actions on a given system. A
Nonlinear Structural Analysis case consists of a
Simulation History, which can contain one or more steps.
Each step represents a period of time in the simulation
history and is associated with a specific analysis
procedure. In the Nonlinear Structural Analysis workbench
you can define the following types of steps:
Inserting a New General Static
Step: Generates a General Static step in a
Nonlinear Structural case. A General Static step is
included by default when you create a Nonlinear
Structural case.
Inserting a New Frequency Step: Generates a
Frequency step in a Nonlinear Structural case.
Inserting a New
General Static Step
Inserting a general static step within the
Simulation History indicates that a static solution
procedure should be used for the computation of the
system response to applied static or quasi-static time
varying loads under given constraints. You can create
environmental specifications (for example, boundary
conditions and loads) within the step. General static
steps are available only in a Nonlinear Structural
case. They can be defined in new analysis cases or in
analysis cases that contain other general static steps;
they cannot be defined in analysis cases that contain
heat transfer steps. However, analysis documents can
contain additional cases with heat transfer steps.
Sequentially coupled thermal-stress analyses, in which
the stress/displacement solution is dependent on a
temperature field but there is no inverse dependency,
can be performed by reading the temperature solution
from a heat transfer analysis case into a stress
analysis case as a predefined field. See
Step Sequence
Restrictions for more information. Nonlinear
Structural Analysis creates a General Static step by
default for a new Nonlinear Structural case.
By default, geometrically nonlinear effects are
considered for general static steps. See
Accounting for Nonlinear Geometric
Effects for more information.
The solver divides a step into increments so that it
can follow the nonlinear solution path. Typically, you
suggest the size of the first increment, and you allow
the solver to choose the size of the subsequent
increments automatically. This approach ensures that
nonlinear problems are solved easily and efficiently.
At the end of each increment the structure is in
(approximate) equilibrium and results are available for
writing to the output database file. Alternatively, you
can specify a fixed increment size that will be used
throughout the step. The latter approach is recommended
only if you have considerable experience with a
particular analysis case.
The ratio of the initial time increment to the total
step time specifies the proportion of load applied in
the first increment. The default initial increment size
is the same as the total time period for the step. As a
result, the solver applies all of the loads defined in
the step in the first increment; if the problem is
linear or mildly nonlinear, the solver will converge to
a solution in a single increment. In contrast, if your
model is highly nonlinear, the solver must reduce the
increment size repeatedly in an attempt to converge to
a solution. You can minimize the time spent reducing
the increment size by providing a reasonable initial
increment size; for most analyses an initial increment
size that is 5% to 10% of the total step time is
sufficient. This value will be modified as required if
automatic incrementation is used or will be used as the
constant time increment if fixed time incrementation is
used.
Note: You can change the
default loading behavior to apply all the loads
instantaneously at the beginning of the step instead
of gradually applying the loads during the step.
However, instantaneous loading may prevent the solver
from reaching a converged solution for models with
significant nonlinearity since reducing the increment
size will no longer correspond to a reduction in the
applied loads.
In some geometrically nonlinear analyses, local
instabilities may occur (e.g., surface wrinkling,
material instability, or local buckling). If the
problem is expected to be unstable, you can choose the
automatic stabilization method available in the solver,
in which damping is applied throughout the model to
prevent instantaneous buckling or collapse.
This task shows you how to insert a new
General Static step in a Nonlinear Structural
case.
-
Select >> from the menu
bar to enter the Nonlinear Structural Analysis
workbench.
-
From the New Analysis Case dialog
box, select Nonlinear Structural
Case.
Nonlinear Structural Analysis creates a
General Static step by default for a new
Nonlinear Structural case.
-
To create an additional General Static step,
do either of the following:
-
To append a new General Static step to the
end of the Simulation History, click the
General Static Step icon .
Tip:
Alternatively, you can select
> from the menu
bar.
-
To insert a new General Static step
between two existing steps in the Simulation
History, right-click the step object in the
specification tree after which you want to
create the new step, then select
> from the menu that
appears.
The General Static Step dialog
box appears, and a new Static Step objects set
appears in the specification tree under the
Simulation History objects set for the current
analysis case.
-
You can change the step identifier by editing
the Step name field. This name
will be used in the specification tree.
-
Enter a description for the step in the
Step
description field.
-
If necessary, do the following to modify the
Basic
Step Data:
-
Edit the Step time field to
specify a value for the total time period
of the step.
-
Specify whether nonlinear geometric
effects should be accounted for in the step
by selecting Off
or On for Nonlinear
geometry. (The default value is
On.) See
Accounting for
Nonlinear Geometric Effects for more information.
-
If necessary, do the following to modify the
Incrementation
Controls:
-
Select the Incrementation type:
Automatic or
Fixed. Automatic
incrementation means that the solver will
select increment sizes based on
computational efficiency. Fixed
incrementation means that you specify a
fixed increment size; this option is
recommended only if you have considerable
experience with a particular analysis
case.
-
Enter a value for the Maximum
number of increments. The
default number of increments for a step is
100; if significant nonlinearity is present
in the simulation, the analysis may require
many more increments. If the solver needs
more increments than the specified upper
limit to complete the step, it will
terminate the analysis with an error
message.
-
Enter a value for the Initial
increment size. The ratio of the
initial time increment to the total step
time specifies the proportion of load
applied in the first increment. The default
initial increment size is the same as the
total time period for the step. As a
result, the solver applies all of the loads
defined in the step in the first increment;
if the problem is linear or mildly
nonlinear, the solver will converge to a
solution in a single increment. In
contrast, if your model is highly
nonlinear, the solver must reduce the
increment size repeatedly in an attempt to
converge to a solution. You can minimize
the time spent reducing the increment size
by providing a reasonable initial increment
size; for most analyses an initial
increment size that is 5% to 10% of the
total step time is sufficient. This value
will be modified as required if automatic
incrementation is used or will be used as
the constant time increment if fixed time
incrementation is used.
-
Enter a value for the Minimum
increment size. This parameter
is used only for automatic time
incrementation. The analysis will terminate
if excessive cutbacks caused by convergence
problems reduce the increment size below
the minimum value.
-
Enter a value for the Maximum
increment size. This parameter
is used only for automatic time
incrementation. By default, there is no
upper limit on the increment size, other
than the total step time. Depending on your
simulation, you may want to specify a
different maximum allowable increment size.
For example, if you know that your
simulation may have trouble obtaining a
solution if too large a load increment is
applied, perhaps because the model may
undergo plastic deformation, you may want
to decrease the maximum increment size.
-
If necessary, do the following to modify the
Stabilization Controls:
-
Click More to access
additional step options.
-
Select Use stabilization to
use automatic stabilization if the problem
is expected to be unstable due to
instabilities caused by localized buckling
behavior or by material instability. Such
instabilities are especially significant
when no time-dependent behavior exists in
the material modeling. the solver can apply
damping throughout the model in such a way
that the viscous forces introduced are
sufficiently large to prevent instantaneous
buckling or collapse but small enough not
to affect the behavior significantly while
the problem is stable.
-
Select the Stabilization
method: Dissipate
Energy Fraction or Damping
Factor.
With the Dissipate Energy
Fraction method, the solver
chooses the damping factor such that the
dissipated energy during the step is a
small fraction of the change in strain
energy during the step.
Alternatively, you can specify the
damping factor directly if you choose the
Damping Factor
method. The damping factor method is
intended for advanced users. You should
define the damping factor directly only in
cases where a certain value is known to be
effective in analyses similar to the
current analysis case.
-
Edit the Stabilization factor
field to specify a value for the
stabilization factor (either the dissipated
energy fraction or the damping factor,
depending on the stabilization method
chosen).
-
If necessary, do the following to modify the
Default
load variation with time:
-
Click More to access
additional step options.
-
Select Instantaneous to
apply all the loads at the start of the
step.
-
Select Ramp linearly over
step (if it is not already
selected) to apply the loads incrementally
over the step.
-
Click OK when you have finished
defining the step.
The Static Step objects set contains a default
Field Output Request object in a Field Output
Requests objects set. See Requesting
Results for more information.

Inserting a New
Frequency Step
Inserting a frequency step within the Simulation
History indicates that an eigenvalue extraction
procedure should be used for the computation of the
system natural frequencies and corresponding mode
shapes. If the frequency step is the first step in the
analysis, initial conditions (for example, temperature)
form the base state for the analysis. Otherwise, the
base state is the current state at the end of the
previous general static step. In a frequency step you
can apply a clamp boundary condition or a displacement
boundary condition with selected degrees of freedom set
to zero; all other boundary conditions and all loads
are ignored. Frequency steps are available only in a
Nonlinear Structural case. They can be defined in new
cases or in cases that contain other general static
steps. Frequency steps cannot be defined in a Thermal
case. See
Step Sequence
Restrictions for more information.
This task shows you how to insert a new
Frequency step in a Nonlinear Structural
case.
-
Select >> from the menu
bar to enter the Nonlinear Structural Analysis
workbench.
-
From the New Analysis Case dialog
box, select Nonlinear Structural
Case.
-
To create an additional Frequency step, do
either of the following:
-
To append a new Frequency step to the end
of the Simulation History, click the
Frequency Step icon .
Alternatively, you can select
> from the menu bar.
-
To insert a new Frequency step between two
existing steps in the Simulation History,
right-click the step object in the
specification tree after which you want to
create the new step, then select
> from the menu that
appears.
The Frequency Step dialog box
appears, and a Frequency Step objects set appears
in the specification tree under the Simulation
History objects set for the current Nonlinear
Structural case.
-
You can change the step identifier by editing
the Step name field. This name
will be used in the specification tree.
-
Enter a description for the step in the
Step
description field.
-
Enter the minimum and maximum frequencies of
interest (Hz). The two values specify a frequency
range within which the solver will calculate
eigenvalues. By default, there is no minimum or
maximum frequency, and the solver calculates the
first ten modes.
-
Choose the Number of modes
requested:
-
If desired, toggle on Frequency
shift and enter a value for the shift
point (Hz2). The eigenvalues closest
to this point will be extracted.
-
Click OK when you have finished
defining the step.
The Frequency objects set contains a default Field
Output Request object in a Field Output Requests
objects set. See Requesting
Results for more information. You cannot
request history output for a frequency step. However,
several whole model history output variables are
generated by default:
-
Eigenfrequency
-
Eigenvalue
-
Effective mass
-
Generalized mass
-
Participation factor
|