Adjoint design sensitivity analysis is used to compute the derivatives of design responses
with respect to one or more design variables. These derivatives are commonly referred to as
sensitivities, because they provide a first-order measure of how sensitive the design response
is to a change in the design variables. The adjoint design sensitivity analysis capability is
useful when the design optimization methodology requires a relatively small set of design
responses, but a large number of design variables, typically one or more variables associated
with each element or node of the design domain. This is the case for topology, sizing, shape,
bead, and ABD stiffness sensitivities, where the adjoint
method for computing design sensitivities is significantly more cost effective computationally
compared to the direct method. More details on the different kinds of structural optimization
methods can be found in About Structural Optimization. However, adjoint sensitivity
analysis can also be used in a stand-alone Abaqus/Standard analysis (that is, outside of an iterative design optimization workflow using Abaqus/Standard and Tosca) to obtain design sensitivities at any stage during the design process.
Material Options
The adjoint sensitivity calculations are supported with elastic, hyperelastic, and
isotropic hardening Mises plasticity material models. With plasticity, the sensitivity
calculations use a total formulation that assumes that the loading is monotonic (that is, no
unloading) and proportional. The sensitivity results are not accurate if the above
assumptions are not valid. More generally, for material constitutive models with
path-dependent and irreversible response, the adjoint sensitivity calculations are supported
only for monotonic loading.
Output
The responses and response sensitivities are output only to the output database
(.odb) file; sensitivity output to the data
(.dat) file and results (.fil) file is not
supported.
The design responses are labeled using the following format:
The
refers to one of the design responses listed in the tables included in
Specifying Design Responses in a Static or an Eigenfrequency Analysis and Specifying Design Responses in a Transient Dynamic Analysis; for example, U1 for the
1-component of the displacement vector at a node, RF2 for
the 2-component of the reaction force vector at a node. The
refers to the name you specified in the design response definition. The
response name helps distinguish among similar design responses.
The labels of the sensitivities are related to the labels of the design responses as
follows:
The
depends on the type of sensitivity analysis as follows:
- For topology sensitivity, the design variable name is prefixed by Abaqus/Standard to be
_density. For example, if the design response
is U1, the corresponding sensitivity is
d_U1_{response_name}__density.
- For shape and bead sensitivities, the design variable name is prefixed by Abaqus/Standard to be
_position. In this case, the sensitivity
output represents a vector with three components in the X-,
Y-, and Z-directions. For example, if the
design response is U1, the corresponding shape or bead sensitivities are a vector
d_U1_{response_name}__position.
- For sizing sensitivity with respect to either the total thickness for noncomposite
shells or an individual layer thickness for composite shells, the design variable name
is prefixed by Abaqus/Standard to be
_thickness.
- For sizing sensitivity with respect to the material orientation angle in a layer of a
composite shell, the design variable name is prefixed by Abaqus/Standard to be
_angle.
- For ABD stiffness sensitivity with respect to the
stiffness components of a shell general section, the design variable name is prefixed by
Abaqus/Standard to be
_stiff. In this case, the sensitivity output
represents a vector with twenty-one components corresponding to the stiffness
components. For example, if the design response is U1, the corresponding
ABD stiffness sensitivities are a vector
d_U1_{response_name}__stiff.
The
in the label for the sensitivities helps distinguish among design
sensitivities that are of the same type.
Limitations
Adjoint design sensitivity analysis is subject to a number of limitations.
- Sizing sensitivity with composite shells and ABD
stiffness sensitivity for shell elements defined using shell general section:
-
- Cannot be used in an eigenfrequency analysis.
- Cannot be used in a direct steady-state dynamic analysis.
- Cannot be used with inertia relief loads.
- Loads and Constraints:
-
- Inertia relief loads are supported only for three-dimensional elements in linear
perturbation steps and load cases.
- Nodes that are involved in a multi-point constraint definition, either as a main
node or a secondary node, cannot be part of the design domain for a shape or bead
sensitivity analysis.
- Topology and sizing design variables cannot be used with the same element in a
linear perturbation static analysis with inertia relief loading.
- Materials:
-
- The isotropic Mises plasticity model is the only supported plasticity material
model. For this model, the sensitivity calculations are based on a total
formulation that assumes that all material points undergo proportional loading
with no unloading.
- For adjoint sensitivity calculations, numerical damping contributions are taken
into account consistently for moderate dissipation or quasi-static applications of
a transient dynamic analysis. While consistent numerical damping contributions are
also included during the adjoint sensitivity calculations of transient fidelity
applications, such problems often experience numerical instabilities during
adjoint sensitivity calculations with thin-walled structures (for example,
shells). In transient dynamic simulations for which the transient fidelity
application type is the default choice, you should use a moderate dissipation
application type for accurate adjoint sensitivities.
- Elements:
-
- Continuum shell elements are not supported for sizing sensitivities.
- The following element types are not supported for shape sensitivities: continuum
elements with incompatible modes; generalized plane strain elements; cylindrical
solid elements; axisymmetric solid elements with nonlinear, asymmetric
deformation; continuum solid shell elements; cylindrical membrane elements; and
axisymmetric membrane elements (with and without twist).
- The following element types are not supported for bead sensitivities: continuum
shell elements; axisymmetric shell elements; axisymmetric shell elements with
nonlinear, asymmetric deformation; conventional three-dimensional shell elements
with five degrees of freedom per node; and triangular facet thin shell elements
(STRI3).
- The internal force design response cannot be associated with elements that have
secondary nodes (for any feature that uses a main-secondary concept, such as a
multi-point constraint).
- Eigenfrequency analysis:
-
- Only the Lanczos or AMS eigensolver can be used
during an eigenfrequency analysis.
- Eigenfrequency response is not available for a preloaded structure.
- Transient analysis:
-
- In a transient dynamic procedure, shape or bead sensitivity analysis is
supported only for moderate dissipation and quasi-static applications.
- A transient dynamic shape sensitivity analysis is not supported for the
following element types: continuum elements with incompatible modes; generalized
plane strain elements; cylindrical solid elements; and axisymmetric solid elements
with nonlinear, asymmetric deformation; continuum solid shell elements;
cylindrical membrane elements; and axisymmetric membrane elements (with or without
twist).
- A transient dynamic bead or shape sensitivity analysis is not supported with
thermal loads.
- A transient dynamic sensitivity analysis must contain only a single dynamic
step.
- For a transient sensitivity analysis, the specification of the time points can
contain only a single time point.
- Material damping is not supported for transient sensitivity calculations.
- For three-dimensional Timoshenko beam elements, a transient sensitivity analysis
supports only isotropic rotary inertia. As a result the rotary inertia associated
with the torsional mode is used for all rotational degrees of freedom.
- Direct steady-state dynamic adjoint sensitivity analysis:
-
- Only supports nodal (translational and rotational) displacement, velocity, and
acceleration responses in sizing, shape, and bead sensitivity analysis. Reaction
forces and moments are not supported as design responses.
- The use of multiple domains is not supported.
- Design-dependent loads and connector elements in the model are not supported.
The node sets specified in the node responses cannot contain any nodes with
dependent degrees of freedom. The aggregation operators over the node sets of the
node responses are limited to sum (default), maximum, and average.
- Preloading and design-dependent loads are not supported.
- Use with restart analyses:
-
- In a restart analysis, you cannot request adjoint design response and
sensitivities if the original analysis did not include such requests.
- You cannot request adjoint design response and sensitivities that are based on
the combined responses of a perturbation step and a preceding general step if the
perturbation step appears in a restart analysis while the preceding general step
appears in the original analysis.
- Static fatigue responses using fe-safe:
-
- Abaqus/Standard supports fatigue design responses for only a static perturbation analysis with
multiple load cases.
- You can include only one fatigue design response type in an Abaqus model. However, you can include several different fatigue responses of the same
type (for example, DAMAGE) but having different
element sets and different design response operators in the same Abaqus model.
- Abaqus/Standard does not support fatigue design response and adjoint sensitivity calculations
for composite sizing (layer thicknesses and angles) design variables.
Input File Template
Input file template for sensitivity analysis in a static procedure:
HEADING
…
NODE, NSET=nset
Data lines to define the nodes
ELEMENT, TYPE=element type, ELSET=elset_elastic
Data lines to define the elements
SOLID SECTION, ELSET=elset_elastic, MATERIAL=elastic
MATERIAL, NAME=elastic
ELASTIC
Data lines to define the elastic properties
STEP, SENSITIVITY=ADJOINT
STATIC
…
DESIGN RESPONSE, NAME=response name
ELEMENT RESPONSE, ELSET=elset name
Data line to specify the element response identifier key
DESIGN RESPONSE, NAME=response name
ELEMENT RESPONSE, ELSET=elset name, NSET=nset name
Data line to specify the element response identifier key
DESIGN RESPONSE, NAME=response name
NODE RESPONSE, NSET=nset
Data line to specify the nodal response identifier key
DESIGN RESPONSE, NAME=response name
GLOBAL RESPONSE
Data lines to specify the global response identifier keys
END STEP
Input file template for sensitivity analysis in a transient dynamic procedure:
HEADING
…
NODE, NSET=nset
Data lines to define the nodes
ELEMENT, TYPE=element type, ELSET=elset_elastic
Data lines to define the elements
SOLID SECTION, ELSET=elset_elastic, MATERIAL=elastic
MATERIAL, NAME=elastic
ELASTIC
Data lines to define the elastic properties
DENSITY
Data lines to define density properties
TIME POINTS, NAME=TimePoint_Name1
Data lines to define a list of time points
TIME POINTS, NAME=TimePoint_Name2
Data lines to define a list of time points
STEP, SENSITIVITY=ADJOINT
DYNAMIC
…
DESIGN RESPONSE, NAME=response name, TIME MARKS=YES, TIME POINTS=TimePoint_Name1
ELEMENT RESPONSE, ELSET=elset name
Data line to specify the element response identifier key
DESIGN RESPONSE, NAME=response name, TIME MARKS=YES, TIME POINTS=TimePoint_Name2
NODE RESPONSE, NSET=nset
Data line to specify the nodal response identifier key
END STEP
Input file template for adjoint sensitivity analysis in a direct steady-state dynamic
procedure:
HEADING
…
NODE, NSET=nset
Data lines to define the nodes
ELEMENT, TYPE=element type, ELSET=elset_elastic
Data lines to define the elements
SOLID SECTION, ELSET=elset_elastic, MATERIAL=elastic
MATERIAL, NAME=elastic
ELASTIC
Data lines to define the elastic properties
DENSITY
Data lines to define density properties
STEP, SENSITIVITY=ADJOINT
STEADY STATE DYNAMICS, DIRECT
…
DESIGN RESPONSE, NAME=response name
NODE RESPONSE, NSET=nset, OPERATOR=operator label, RANGE OPERATOR=range operator label
Data line to specify the nodal response identifier key
frequency lower limit, frequency upper limit
END STEP
Input file template for fatigue design sensitivity analysis:
HEADING
…
NODE, NSET=nset
Data lines to define the nodes
ELEMENT, TYPE=element type, ELSET=elset_elastic
Data lines to define the elements
SOLID SECTION, ELSET=elset_elastic, MATERIAL=elastic
MATERIAL, NAME=elastic
ELASTIC
Data lines to define the elastic properties
STEP, PERTURBATION SENSITIVITY=ADJOINT
STATIC
…
LOAD CASE, NAME=name1
…
END LOAD CASE
LOAD CASE, NAME=name2
…
END LOAD CASE
…
DESIGN RESPONSE, NAME=response name
ELEMENT RESPONSE, FATIGUE, ELSET=elset name
Data line to specify the element response identifier key
END STEP
|