Adjoint Design Sensitivity Analysis

Adjoint Sensitivity Method for Transient Dynamics Using Abaqus/Standard

The adjoint sensitivity approach for transient dynamic problems is based on the implicit dynamic procedure in Abaqus/Standard. Some classes of problems are better suited than others for such an approach. These problems include low frequency–mode bending-dominated deformations and low-velocity crash problems (such as side crashes and other bending-dominated crashes). Other problems in this category include battery frame crashes, pedestrian head impacts, dynamics of machinery, and compliant flexible dynamic mechanisms. Typically, such problems use 30–300 increments to capture the correct physics and applying Abaqus/Standard is appropriate. Therefore, the adjoint sensitivity method for transient dynamics is applicable for these situations.

However, for high frequency–mode crash problems (for example, axial deformation and crushing), very small time increments are required to capture the correct physics. The run time for many practical applications of this latter type are not feasible for Abaqus/Standard due to a very large number of time increments. Therefore, Abaqus/Explicit is better suited to solve this class of problems. Also, Abaqus/Standard might often fail to converge when the models have significant nonlinearities (many contacts and many buckling modes). Such problems are also solved more effectively using Abaqus/Explicit.

Activating Adjoint Sensitivity Analysis

You activate an adjoint sensitivity analysis on a step-by-step basis.

Input File Usage

Use the following option to activate an adjoint sensitivity analysis in a particular step:

STEP, SENSITIVITY=ADJOINT

Activating Adjoint Sensitivity Analysis in Multiple Steps

If you activate an adjoint sensitivity calculation in any general step during the analysis, it is activated for all general steps in the analysis, including steps before the activating step. Likewise, if you activate an adjoint sensitivity calculation in any perturbation step during the analysis, it is activated for all perturbation steps in the analysis, including steps before the activating step. In both of these situations, the sensitivity calculations occur for any given step that includes responses. In a linear perturbation step with multiple load cases, the design sensitivity calculations are carried out for all the load cases. The adjoint sensitivity calculations cannot be selectively deactivated for some of the load cases.

Specifying Design Variables

Unlike direct design sensitivity analysis (which is commonly used for parametric design and optimization), adjoint design sensitivity analysis is commonly used for nonparametric design and optimization. The design parameters are more commonly referred to as design variables in this case. Unlike direct design sensitivity analysis (where the number of design parameters is relatively small in number), an adjoint design sensitivity analysis typically has one or more design variables associated with each element in the design domain.

The specific choices for design variables depend on the type of design sensitivities that you desire, as listed in the table below. For topology and sizing sensitivities, the design variables and the corresponding design sensitivities are element-based, while for shape and bead sensitivities these quantities are node-based.


Type of sensitivity	Design variables
Topology	Relative material density
Sizing for non-composite shells	Shell element thickness
Sizing for circular section beams	Beam element radius
Shape or bead	Nodal positions
Sizing for composite shells	Composite layer thickness and/or orientation

Topology Sensitivity

The design variables for topology optimization are the material relative densities for the elements in the design domain. The material relative density is a nondimensional quantity that can take a value that is greater than 0 but less than or equal to 1. A value of 1 corresponds to the original material density, while a value that is close to 0 corresponds to removal of material to create a void. For computing design response and sensitivities, Abaqus/Standard makes use of scaling factors and their derivatives for stiffness, mass, and stress design response, respectively. The scaling factors and their derivatives are all functions of the relative material density, and you can use a spatial distribution to specify them directly. All elements in the design domain must explicitly specify a value for the different scaling factors and their derivatives as part of the spatial distribution definition. An element for which the scaling factors and its derivatives are not specified is assumed not to be a part of the design domain.

Input File Usage

Use the following options to define the stiffness scaling factors and their derivatives for topology sensitivities:

SCALE STIFFNESS
distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the mass scaling factors and their derivatives for topology sensitivities:

SCALE MASS
distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the stress design response scaling factors and their derivatives for topology sensitivities:

SCALE STRESS DESIGN
distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Sizing Sensitivity with Non-Composite Shell Elements

The design variables for sizing with non-composite shell elements are the shell thicknesses. All elements in the design domain must explicitly specify a value for the shell thickness using a spatial distribution. An element for which the thickness is not specified in the spatial distribution definition is assumed not to be a part of the design domain.

Input File Usage

Use the following options to define the design variables for sizing sensitivity for shell elements with the section behavior integrated during the analysis:

SHELL SECTION, SHELL THICKNESS=distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the design variables for sizing sensitivity for shell elements with general section behavior:

SHELL GENERAL SECTION, SHELL THICKNESS=distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Sizing Sensitivity with Composite Shell Elements

The design variables for sizing with composite shell elements are the composite layer thicknesses and the orientation angles. All elements in the design domain must explicitly specify a value for the layer thickness and/or orientation angle using spatial distributions. If you do not specify the layer thickness or orientation angle in the spatial distribution definition for an element, Abaqus/Standard assumes that element is not part of the design domain.

Input File Usage

Use the following options to define the design variables for the layer sizing for composite shell elements with the section behavior integrated during the analysis:

SHELL SECTION, COMPOSITE 
distribution name, number of integration points, name of the material forming this layer, orientation of this layer
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the design variables for the layer sizing for composite shell elements with general section behavior:

SHELL GENERAL SECTION, COMPOSITE
distribution name, , name of the material forming this layer, orientation of this layer
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the design variables for the layer orientation angle for composite shell elements with the section behavior integrated during the analysis:

SHELL SECTION, COMPOSITE 
layer thickness, number of integration points, name of the material forming this layer, distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Use the following options to define the design variables for the layer orientation angle for composite shell elements with general section behavior:

SHELL GENERAL SECTION, COMPOSITE
layer thickness, , name of the material forming this layer, distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Sizing Sensitivity with Circular Section Beam Elements

The design variables for sizing with circular section beam elements are the beam radii. All elements in the design domain must explicitly specify a value for the beam radius using a spatial distribution. An element for which the radius is not specified in the spatial distribution definition is assumed not to be a part of the design domain. Adjoint design sensitivity calculations with circular section beams is supported only for elements with section behaviors that are integrated during the analysis.

You must request output variable BRADIUS, which contains the beam radius for a circular cross-section beam, to render (visualize) the beam elements with varying radii properly in the Visualization module of Abaqus/CAE. Otherwise, all beam radii are rendered with a value of 1.0.

Input File Usage

Use the following options to define the design variables for sizing optimization with circular section beam elements:

BEAM SECTION, SECTION=CIRC
distribution name
DISTRIBUTION, LOCATION=ELEMENT, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Shape Sensitivity with Solid Elements

The design variables for shape sensitivity analysis with solid elements are the positions (coordinates) for all nodes that are in the design domain. All nodes in the design domain must explicitly specify, as part of a spatial distribution, a value of the displacement components relative to their original locations. A node for which the displacement is not specified through a spatial distribution definition is assumed to not be a part of the design domain.

Input File Usage

Use the following options to define the design variables for shape optimization with solid elements:

ADJUST, DISTRIBUTION=distribution name, NODE SET=name
DISTRIBUTION, LOCATION=NODE, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Bead Sensitivity with Shell Elements

The design variables for a bead sensitivity analysis with shell elements are the positions (coordinates) of all nodes that are in the design domain. All nodes in the design domain must explicitly specify, as part of a spatial distribution, a value of the displacement components relative to their original locations. A node for which the displacement is not specified through a spatial distribution definition is assumed to not be a part of the design domain.

Input File Usage

Use the following options to define the design variables for bead optimization with shell elements:

ADJUST, DISTRIBUTION=distribution name, NODE SET=name
DISTRIBUTION, LOCATION=NODE, DESIGN VARIABLE, NAME=distribution name, TABLE=distribution table name
DISTRIBUTION TABLE, NAME=distribution table name

Specifying Design Responses in a Static or an Eigenfrequency Analysis

An adjoint design sensitivity analysis supports three kinds of design responses: element responses, global responses, and node responses. The valid element responses are von Mises stress, signed von Mises stress (the sign of this quantity is the same as the sign of the trace of the stress tensor), maximum principal stress, minimum principal stress, plastic strain magnitude, Neuber and Glinka plasticity correction quantities (Plasticity Corrections), a user-defined response based on either the stress or the plastic strain, and internal forces. A stress- or plastic strain–based design response represents a scalar measure calculated using a specified operator (by default, the maximum) on the values in the specified element set. Abaqus/Standard uses the stresses or the plastic strains at the element integration points to compute stress- or plastic strain–based design responses and sensitivities. The internal forces response represents a scalar measure calculated using a specified operator (by default, the sum) on the internal nodal forces over a set of specified nodes from a specified set of elements.

For a user-defined design response based on stress or plastic strain, you must define the design response in user subroutine UELEMDRESP (see Defining the Design Response in User Subroutine UELEMDRESP).

Only two types of global responses are available: stiffness and eigenfrequency. The global stiffness response, available in a static procedure, provides a measure of the stiffness of the structure that accounts for both external loading and prescribed displacements. It is defined as

G_{s t i f f} = \frac{1}{2} P \cdot U - \frac{1}{2} R_{F} \cdot U_{p r e s},

where $P$ , $U$ , $R_{F}$ , and $U_{p r e s}$ refer to vectors representing external loads, displacements, reaction forces, and prescribed displacements on the structure. For a structure that has only external loading and no prescribed displacements, the second term is identically zero, and only the first term produces a nonzero contribution. The global eigenfrequency response, available in an eigenfrequency procedure, refers to one or more eigenfrequencies of the structure.

The node responses refer to quantities such as displacements or reaction forces and moments at one or more nodes in the structure.

You request design responses using a syntax analogous to that for specifying output requests to the output database. There are no default responses. If no responses are requested, no design responses and no sensitivities are output. Specifying a response outputs both the design response value and the response sensitivities.

For internal forces and internal moments in element responses, both an element and a node set must be specified to define the design response. Each node in the specified node set receives contributions from all the elements in the specified element set that are attached to it. For element responses and node responses, if the node set contains more than one node, the design response contains the sum of the contributions from all the nodes in the node set.

By default, the sensitivity for the stress and the plastic strain magnitude responses are approximated with aggregation functions over the specified element set, where the default is an aggregation function representing the maximum. Other aggregation functions approximating the minimum and the difference between the maximum and minimum values are also available. You apply these operator types for the design response. Additional operators for elemental design responses are the sum and the average over the elemental integration points of a given element set.

Input File Usage

Use the following options to request element design responses:

DESIGN RESPONSE, NAME=response name
ELEMENT RESPONSE, ELSET=elset name, NSET=nset name, ORIENTATION=orientation name, OPERATOR=operator name

Use the following options to request global design responses:

DESIGN RESPONSE, NAME=response name
GLOBAL RESPONSE

Use the following options to request node design responses:

DESIGN RESPONSE, NAME=response name
NODE RESPONSE, NSET=nset name, ORIENTATION=orientation name

Each design response specification block must only request a single design response. Multiple design responses require multiple uses of the design response specification block, once for each response.

Defining the Design Response in User Subroutine UELEMDRESP

For a user-defined element design response based on stress or plastic strain, you must define the design response in user subroutine UELEMDRESP. You specify an element response identifier label (such as TRESCA, MISES_PE, or DRESP_1), the name of a table collection that refers to a property or parameter table, and output variable S or PE. The specified table collection is activated before the user subroutine is called. If no table collection is specified, Abaqus activates the table collection, if any, that is associated with the material definition of the elements in the design domain.

Input File Usage

Use the following options to define the element design response in user subroutine UELEMDRESP:

DESIGN RESPONSE, NAME=response_name
ELEMENT RESPONSE, USER, ELSET=elset_name
element response identifier label, table collection name, output variable identifier

For example, the following input defines a Tresca stress invariant as the element design response:

DESIGN RESPONSE, NAME=response_name
ELEMENT RESPONSE, USER, ELSET=E1
TRESCA, TC_NAME, S

Requesting Responses in Multiple Steps

Unless specified otherwise, response requests defined in a step propagate to subsequent steps according to the following rules:

Requests in general steps propagate to subsequent general steps.
Requests in linear perturbation steps propagate to subsequent consecutive linear perturbation steps.

Responses in a Linear Static Perturbation Step

For sensitivities in a static linear perturbation step following a general static step, the design responses are computed based on the total values of the appropriate physical quantities. Here, total refers to the sum of the physical quantities from the general and the perturbation steps. This approach is particularly useful when the general step represents the preloading and the assembly process of a structure while the perturbation step, which is typically composed of a number of load cases, represents service and live loads. The perturbation step may or may not apply the Linear Complementarity Problem (LCP) solution technique (see Linear Complementarity Problem (LCP) Solution Technique for Solving Contact Problems).

Restrictions on Responses

The tables below describe the available design responses for various procedure types.


Procedure type	Physical quantity	Node response
Static	Displacement components	U1, U2, U3
	Displacement magnitude	UMAG
	Rotation components	UR1, UR2, UR3
	Rotation magnitude	URMAG
	Reaction force components	RF1, RF2, RF3
	Reaction force magnitude	RFMAG
	Reaction moment components	RM1, RM2, RM3
	Reaction moment magnitude	RMMAG


Procedure type	Physical quantity	Element response
Static	Internal force components	INTF1, INTF2, INTF3
	Internal force magnitude	INTFMAG
	Internal moment components	INTM1, INTM2, INTM3
	Internal moment magnitude	INTMMAG
	Von Mises equivalent stress	MISES
	Signed von Mises equivalent stress	S_MISES
	Maximum principal stress	SP3
	Minimum principal stress	SP1
	Neuber equivalent stress	NBSEQ
	Glinka equivalent stress	GKSEQ
	Neuber equivalent strain	NBEEQ
	Glinka equivalent strain	GKEEQ
	Plastic strain magnitude	PEMAG
	Neuber equivalent plastic strain	NBPEEQ
	Glinka equivalent plastic strain	GKPEEQ


Procedure type	Physical quantity	Global response
Static	Global stiffness measure	STIFF
Frequency	Eigenfrequency	FREQ

Specifying Design Responses in a Transient Dynamic Analysis

A transient dynamic adjoint design sensitivity analysis supports two kinds of design responses: node responses and element responses. The node responses refer to quantities such as displacements or reaction forces and moments at one or more nodes in the structure. Most of the available responses are node responses; the only valid element response is internal rate of work (power flow) for a given element set.

You request design responses using a syntax analogous to that for specifying output requests to the output database. There are no default responses. If no responses are requested, no design responses and no sensitivities are output. Specifying a response outputs both the design response value and its sensitivities. You must specify a node set or an element set as part of a node or an element design response definition. If the set contains more than one entity (node or element), the design response contains the sum of the contributions from all of the entities in the set.

Optionally, you can specify one or more time points at which a physical quantity of interest is to be treated as a design response. If no time point is specified, the time point corresponding to the end of the step is used for the design response.

Input File Usage

Use the following options to request element design responses at a specific time point:

DESIGN RESPONSE, NAME=response name, TIME MARKS=YES, TIME POINTS=time point name
ELEMENT RESPONSE, ELSET=elset name

Use the following options to request node design responses at a specific time point:

DESIGN RESPONSE, NAME=response name, TIME MARKS=YES, TIME POINTS=time point name
NODE RESPONSE, NSET=nset name, ORIENTATION=orientation name

Each design response specification block must request only a single design response. Multiple design responses require multiple uses of the design response specification block, once for each response.

Restrictions on Responses

The tables below describe the available design responses for a transient dynamic procedure.


Procedure type	Physical quantity	Node response
Transient dynamic	Displacement components	U1, U2, U3
	Displacement magnitude	UMAG
	Rotation components	UR1, UR2, UR3
	Rotation magnitude	URMAG
	Translational velocity components	V1, V2, V3
	Translational velocity magnitude	VMAG
	Rotational velocity components	VR1, VR2, VR3
	Rotational velocity magnitude	VRMAG
	Translational acceleration components	A1, A2, A3
	Translational acceleration magnitude	AMAG
	Rotational acceleration components	AR1, AR2, AR3
	Rotational acceleration magnitude	ARMAG
	Reaction force components	RF1, RF2, RF3
	Reaction moment components	RM1, RM2, RM3


Procedure type	Physical quantity	Element response
Transient dynamic	Rate of internal work	ELPF

Specifying Design Responses in a Direct Steady-State Dynamic Analysis

A direct steady-state dynamic adjoint design sensitivity analysis supports only node responses for sizing optimization with non-composite shell elements and circular-section beam elements. The node responses refer to quantities such as displacements, velocities, or accelerations at one or more nodes in the structure. For each design response, you specify a range of frequencies over which the sensitivities are computed. The output values of a design response and the corresponding sensitivities are aggregates (default is maximum) computed over the range of frequencies specified for the design response.

There are no default responses. If no responses are requested, no design responses and no sensitivities are output. Specifying a response outputs both the design response value and its sensitivities. You must specify a node set for each node response requested. If the node set has multiple nodes, the design response contains the aggregate (default is sum) of the contributions from all of the nodes in the node set.

The frequency range, which you specify with a node response request, must include one or more frequency values at which the primal steady-state dynamic response is computed. If this is not the case, Abaqus/Standard outputs the design response and sensitivities as zeros. You may also obtain the primal steady-state dynamic response at frequency values that are outside of the range specified with the node response definition; these have no effect on the design response and sensitivity output.

The node set you specify for any node response should not contain any node with a dependent degree of freedom. There should be no preloading in an analysis with a direct steady-state dynamic adjoint design sensitivity analysis step. Connector elements and design dependent loads (such as gravity loading, GRAV) are not supported in a direct steady-state dynamic adjoint design sensitivity analysis. You can run a direct steady-state dynamic analysis on multiple domains; however, if you request an adjoint sensitivity analysis for this procedure, you can run the analysis only on a single domain. The permitted aggregation operators over the node set are sum (SUM), maximum (MAX), and average (AVE).

Input File Usage

Use the following options to request a node design response over a frequency range:

DESIGN RESPONSE, NAME=response name
NODE RESPONSE, NSET=nset name, OPERATOR=operator label, RANGE OPERATOR=range operator label
node response label
frequency range lower limit, frequency range higher limit

Each design response specification block must request only a single design response. Multiple design responses require multiple uses of the design response specification block, once for each response.

Restrictions on Responses

The table below describes the available design responses for a direct steady-state dynamic procedure.


Procedure type	Physical quantity	Node response
Direct steady-state dynamic	Displacement components	U1, U2, U3
	Displacement magnitude	UMAG
	Rotation components	UR1, UR2, UR3
	Rotation magnitude	URMAG
	Velocity components	V1, V2, V3
	Velocity magnitude	VMAG
	Rotational velocity components	VR1, VR2, VR3
	Rotational velocity magnitude	VRMAG
	Acceleration components	A1, A2, A3
	Acceleration magnitude	AMAG
	Rotational acceleration components	AR1, AR2, AR3
	Rotational acceleration magnitude	ARMAG

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 utilizing the following format:

DResp_{r e s p o n s e_i d e n t i f i e r}_{r e s p o n s e_n a m e}

The $r e s p o n s e_i d e n t i f i e r$ 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 $r e s p o n s e_n a m e$ 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:

d_{r e s p o n s e_i d e n t i f i e r}_{r e s p o n s e_n a m e}_{d e s i g n_v a r i a b l e_n a m e}

The $d e s i g n_v a r i a b l e_n a m e$ depends on the type of sensitivity analysis. 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 non-composite 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. The $r e s p o n s e_n a m e$ in the label for the sensitivities helps distinguish among design sensitivities that are of the same type.

Limitations

Adjoint design sensitivity analysis are subject to a number of limitations.

Sizing sensitivity with composite shells:

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.

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 eigensolver can be used during an eigenfrequency analysis.

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 hybrid, modified, and incompatible-mode elements as design elements, but these elements can be present in the model.
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:

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 is 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.

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