Limitations
Currently frequency responses are allowed only for sizing
optimization.
Options in Context of Frequency Response
The following lists which options can be applied in frequency response optimization using Tosca Structure and Abaqus:
- The following types of analysis are supported in
Abaqus:
*STEADY STATE DYNAMICS, DIRECT
*STEADY STATE DYNAMICS, SUBSPACE PROJECTION
*STEADY STATE DYNAMICS
(The modal superposition is used in
Abaqus
when DIRECT or SUBSPACE PROJECTION is not defined.)
- The excitation frequencies should always stay constant during the
optimization iterations. Consequently, the locations of the excitation
frequencies determined from the eigenfrequencies (an option in modal analysis)
are prohibited. The following ways of defining excitation frequencies exist in
Abaqus:
- For
DIRECT and analysis SUBSPACE PROJECTION :
INTERVAL=RANGE is allowed (default for DIRECT ).
INTERVAL=EIGENFREQUENCY is not allowed (default for SUBSPACE PROJECTION ).
- Modal analysis:
INTERVAL=RANGE is allowed.
INTERVAL=EIGENFREQUENCY is allowed.
- When
*STEADY STATE DYNAMICS, DIRECT is applied, all
requests that Tosca Structure
requires from Abaqus
for the optimization are not available from the *STEP containing
*STEADY STATE DYNAMICS, DIRECT . However, these can
be requested in the eigenfrequency extraction analysis. Consequently, an
eigenfrequency extraction (modal analysis) should always be applied before the
STEADY STATE DYNAMICS, DIRECT analysis. This can be
done without much CPU effort by defining the following as the first
*STEP in the Abaqus finite element input file:
*STEP
*FREQUENCY, EIGENSOLVER=LANCZOS, NORMALIZATION=MASS
1, 0.0, ,
*END STEP
- Only pure linear frequency responses are supported. Thus, no
prestress (stress stiffening) before the frequency is allowed.
- The normalization option
MASS will be used by default. It will be set
automatically regardless of the original option.
- Prescribed displacements, velocities, and accelerations for
Abaqus
are supported in frequency response using the command
*BOUNDARY including one or several of the following
arguments:
TYPE=DISPLACEMENT
TYPE=VELOCITY
TYPE=ACCELERATION
Other types of prescribed displacements, velocities, and
accelerations for Abaqus are not supported for frequency response.
- The geometric nonlinearities and the incompatible, modified, and hybrid elements are not
supported as design elements (
DV_TOPO ) for frequency response. Elements, which
are allowed as design elements (DV_TOPO ) in frequency response, are marked
with an ’F’ in the table of supported element types ( Supported Element Types), but all other elements are allowed outside the design area.
Damping
The following lists the options to deal with dumping:
- For
DIRECT and analysis SUBSPACE PROJECTION :
- For modal superposition procedures:
|