김경종
176 lines
14 KiB
Markdown
176 lines
14 KiB
Markdown
<!-- source-page: 1451 -->
|
||
|
||
• GETWAVE determines wave kinematic data associated with the applied wave theory in an Abaqus/Aqua analysis (“Obtaining wave kinematic data in an Abaqus/Aqua analysis,” Section 2.1.13 of the Abaqus User Subroutines Reference Guide).
|
||
GETWAVEVEL, GETWINDVEL, and GETCURRVEL are used to obtain the wave, wind, and steady current velocity components, respectively, for a given point in an Abaqus/Aqua analysis (“Obtaining wave kinematic data in an Abaqus/Aqua analysis,” Section 2.1.13 of the Abaqus User Subroutines Reference Guide).
|
||
• STDB\_ABQERR or XPLB\_ABQERR can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to print an informational, warning, or error message to the message file in Abaqus/Standard or the status file in Abaqus/Explicit (“Printing messages to the message or status file,” Section 2.1.14 of the Abaqus User Subroutines Reference Guide).
|
||
• XIT or XPLB\_EXIT can be called from any Abaqus/Standard or Abaqus/Explicit user subroutine, respectively, to terminate an analysis (“Terminating an analysis,” Section 2.1.15 of the Abaqus User Subroutines Reference Guide).
|
||
• IGETSENSORID or IVGETSENSORID can be called from Abaqus/Standard user subroutine UAMP or Abaqus/Explicit user subroutine VUAMP, respectively, to obtain the ID of a user-defined sensor. GETSENSORVALUE or VGETSENSORVALUE can be called from Abaqus/Standard user subroutine UAMP or Abaqus/Explicit user subroutine VUAMP, respectively, to obtain the value of a user-defined sensor (“Obtaining sensor information,” Section 2.1.16 of the Abaqus User Subroutines Reference Guide).
|
||
• MATERIAL\_LIB\_MECH can be called from Abaqus/Standard user subroutine UELMAT to access the Abaqus material library (“Accessing Abaqus materials,” Section 2.1.17 of the Abaqus User Subroutines Reference Guide).
|
||
• MATERIAL\_LIB\_HT can be called from Abaqus/Standard user subroutine UELMAT to access the Abaqus thermal material library (“Accessing Abaqus thermal materials,” Section 2.1.18 of the Abaqus User Subroutines Reference Guide).
|
||
• SMACfdUserSubroutineGetScalar can be called from any Abaqus/CFD user subroutine to access selected output variables for elements or surface facets that are part of a boundary condition definition (“Obtaining scalar state information in an Abaqus/CFD analysis,” Section 2.1.19 of the Abaqus User Subroutines Reference Guide).
|
||
• SMACfdUserSubroutineGetVector can be called from any Abaqus/CFD user subroutine to access selected output variables for elements and surface facets that are part of a boundary condition definition (“Obtaining vector state information in an Abaqus/CFD analysis,” Section 2.1.20 of the Abaqus User Subroutines Reference Guide).
|
||
• SMACfdUserSubroutineGetMpiComm can be called from within any Abaqus/CFD user subroutine to obtain the MPI communicator used in a parallel analysis job (“Obtaining the MPI communicator in an Abaqus/CFD analysis,” Section 2.1.21 of the Abaqus User Subroutines Reference Guide).
|
||
• MutexInit, MutexLock, and MutexUnlock can be used to create and manipulate mutexes (“Ensuring thread safety,” Section 2.1.22 of the Abaqus User Subroutines Reference Guide).
|
||
|
||
<!-- source-page: 1452 -->
|
||
|
||
• Dynamically allocatable arrays can be used to accumulate and store data. All basic types are supported. In addition, Abaqus provides arrays of type Real that change precision automatically (“Allocatable arrays,” Section 2.1.23 of the Abaqus User Subroutines Reference Guide).
|
||
|
||
– Real arrays will run in single precision when Abaqus/Explicit runs in single precision and will run in double precision when Abaqus/Explicit runs in double precision.
|
||
– Arrays of structures can be used to store data of any user-defined type, including Fortran and C/C++ structures and classes with arbitrary sizes and number of fields.
|
||
|
||
• Thread-local arrays can be used to allocate storage local to a thread. SMALocalIntArrayCreate and SMALocalFloatArrayCreate can be used to create or resize a local array. SMALocalIntArrayAccess and SMALocalFloatArrayAccess can be used to locate an existing local array. SMALocalIntArrayDelete and SMALocalFloatArrayDelete can be used to delete a local array. SMALocalIntArraySize and SMALocalFloatArraySize can be used to get the size of the array (“Allocatable arrays,” Section 2.1.23 of the Abaqus User Subroutines Reference Guide).
|
||
|
||
• Global arrays can also be used to allocate storage shared among all threads. SMAIntArrayCreate and SMAFloatArrayCreate can be used to create or resize a global array. SMAIntArrayAccess and SMAFloatArrayAccess can be used to locate an existing global array. SMAIntArrayDelete and SMAFloatArrayDelete can be used to delete a global array. SMAIntArraySize and SMAFloatArraySize can be used to get the size of the global array (“Allocatable arrays,” Section 2.1.23 of the Abaqus User Subroutines Reference Guide).
|
||
|
||
<!-- source-page: 1453 -->
|
||
|
||
# 19. Design Sensitivity Analysis
|
||
|
||
Design sensitivity analysis
|
||
|
||
<!-- source-page: 1454 -->
|
||
|
||
<!-- source-page: 1455 -->
|
||
|
||
# 19.1 Design sensitivity analysis
|
||
|
||
• “Design sensitivity analysis,” Section 19.1.1
|
||
|
||
<!-- source-page: 1456 -->
|
||
|
||
<!-- source-page: 1457 -->
|
||
|
||
# 19.1.1 DESIGN SENSITIVITY ANALYSIS
|
||
|
||
Product: Abaqus/Design
|
||
|
||
# References
|
||
|
||
• “Parametric input,” Section 1.4.1
|
||
• “Parametric shape variation,” Section 2.1.2
|
||
• \*STEP
|
||
• \*DESIGN PARAMETER
|
||
• \*DESIGN RESPONSE
|
||
|
||
# Overview
|
||
|
||
Design sensitivity analysis (DSA):
|
||
|
||
• is performed with Abaqus/Design, an add-on option for Abaqus/Standard;
|
||
• provides the sensitivities of responses with respect to specified design parameters;
|
||
• is available for static stress and frequency analysis using models that have only stress/displacement elements; and
|
||
• can include design parameters affecting: material properties (elastic, hyperelastic, and hyperfoam models); section properties; concentrated forces and moments; and nodal coordinates (and beam and shell normals if applicable).
|
||
|
||
# Design sensitivity analysis
|
||
|
||
The design sensitivity analysis (DSA) capability provides the derivatives of certain output variables with respect to specified design parameters. These derivatives are commonly referred to as sensitivities, because they provide a first-order measure of how sensitive the output variable is to a change in the design parameter. The output variables for which sensitivities are computed are called design responses or simply responses. Design parameters are chosen from a set of existing analysis parameters. As an example, you can choose to obtain the derivatives of stresses with respect to Young’s modulus; stress is the response, and Young’s modulus is the design parameter. The sensitivities are computed based on the direct differentiation method used in conjunction with the semi-analytical computational technique. In the semi-analytical technique some derivatives are computed using numerical (finite) differencing, thus requiring perturbations of the design parameters. For these derivatives by default Abaqus/Design will use a central differencing scheme and automatically determine appropriate perturbation sizes based on a heuristic algorithm. You can override these defaults by specifying the numerical differencing method and the perturbation sizes directly. A full discussion of DSA theory is given in “Design sensitivity analysis,” Section 2.18.1 of the Abaqus Theory Guide.
|
||
|
||
<!-- source-page: 1458 -->
|
||
|
||
# Activating DSA
|
||
|
||
You activate DSA on a step-by-step basis.
|
||
|
||
Input File Usage: Use the following option to activate DSA in a particular step: \*STEP, DSA=YES
|
||
|
||
# Activating DSA in multiple steps
|
||
|
||
Once DSA is activated in a general step, it remains active in all subsequent general steps until it is deactivated in a subsequent general step. Once DSA is activated in a perturbation step, it remains active in all subsequent consecutive perturbation steps until it is deactivated in a subsequent consecutive perturbation step. However, if DSA is activated in a step whose procedure is not supported for DSA, DSA will be deactivated until it is activated again.
|
||
|
||
Input File Usage: Use the following option to deactivate DSA in a particular step: \*STEP, DSA=NO
|
||
|
||
# Specifying design parameters
|
||
|
||
You can define multiple parameters to be used in place of Abaqus input quantities for an analysis. You must indicate which of these parameters are to be considered as design parameters.
|
||
|
||
Input File Usage: Use the following option to define analysis parameters: \*PARAMETER par1=x par2=y Use the following option to specify the design parameters: \*DESIGN PARAMETER par1, par2,
|
||
|
||
# Restrictions on design parameters
|
||
|
||
The following are restrictions on design parameters:
|
||
|
||
• Design parameters can be associated only with floating point data. The following analysis components can include design-dependent data:
|
||
– Beam sections integrated during analysis (“Using a beam section integrated during the analysis to define the section behavior,” Section 29.3.6)
|
||
– Concentrated loads (“Concentrated loads,” Section 34.4.2)
|
||
– Elastic materials (“Linear elastic behavior,” Section 22.2.1)
|
||
– Friction (“Frictional behavior,” Section 37.1.5)
|
||
– Gasket sections (“Gasket elements: overview,” Section 32.6.1)
|
||
– Hyperelastic materials (“Hyperelastic behavior of rubberlike materials,” Section 22.5.1)
|
||
|
||
<!-- source-page: 1459 -->
|
||
|
||
– Hyperfoam materials (“Hyperelastic behavior in elastomeric foams,” Section 22.5.2)
|
||
– Membrane sections (“Membrane elements,” Section 29.1.1)
|
||
– Local orientations (“Orientations,” Section 2.2.5)
|
||
– Shell sections integrated during analysis (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5)
|
||
– Solid sections (“Solid (continuum) elements,” Section 28.1.1)
|
||
– Transverse shear stiffnesses (“Choosing a beam element,” Section 29.3.3, or “Shell section behavior,” Section 29.6.4)
|
||
|
||
• Shape design parameters (i.e., design parameters that affect nodal coordinates and beam and/or shell normals) can be used only in conjunction with parametric shape variations (see “Parametric shape variation,” Section 2.1.2).
|
||
• Design parameters must be mutually independent.
|
||
• Design parameters cannot be tabularly dependent (see “Parametric input,” Section 1.4.1).
|
||
|
||
# Specifying responses
|
||
|
||
Response requests are specified using a syntax analogous to that for specifying output requests to the output database. Except for eigenvalues and eigenfrequencies, there are no default responses—if no responses are requested, no response sensitivities will be output. If DSA is active in a frequency step, eigenvalue and eigenfrequency sensitivities will be output automatically. Specifying a response will cause output of both the response and the response sensitivities.
|
||
|
||
Input File Usage: Use the following options to request design responses:
|
||
|
||
\*DESIGN RESPONSE, FREQUENCY=interval, MODE LIST
|
||
|
||
\*CONTACT RESPONSE, MASTER=master name, NSET=nset name,
|
||
|
||
SLAVE=slave name
|
||
|
||
\*ELEMENT RESPONSE, ELSET=elset name
|
||
|
||
\*NODE RESPONSE, NSET=nset name
|
||
|
||
# Requesting responses in multiple steps
|
||
|
||
Unless respecified, response requests defined in a step propagate to subsequent steps according to the following rules:
|
||
|
||
1. Requests in general steps propagate to subsequent general steps.
|
||
2. Requests in linear perturbation steps propagate to subsequent consecutive linear perturbation steps.
|
||
3. When a non-DSA step appears between DSA steps, the responses must be respecified in the DSA step following the non-DSA step.
|
||
|
||
# Restrictions on responses
|
||
|
||
The available responses are a subset of the existing output variables. The valid responses based on procedure type are described below.
|
||
|
||
<!-- source-page: 1460 -->
|
||
|
||
• For static steps the valid responses are:
|
||
|
||
– Node responses: U and RF
|
||
– Element responses: S, SF, SINV, SP, E, SE, EP, EE, EEP, LE, LEP, NE, NEP, ENER, ELEN, EVOL, and MASS
|
||
– Contact responses: CSTRESS and CDISP
|
||
|
||
• For frequency steps the valid responses are:
|
||
|
||
– Node responses: None
|
||
– Element responses: MASS
|
||
– Contact responses: None
|
||
– Eigenvalue (EIGVAL) and eigenfrequency (EIGFREQ) sensitivities are output automatically.
|
||
|
||
# Specifying design gradients of design-dependent input data
|
||
|
||
The DSA calculations require the gradients of the design-dependent input data with respect to the design parameters. For example, if Poisson’s ratio, , is made dependent on a design parameter, say h, the gradient is required. Design gradients with respect to shape design parameters are specified differently than those with respect to other design parameters.
|
||
|
||
# Specifying design gradients with respect to shape design parameters
|
||
|
||
Gradients with respect to shape design parameters must be specified using a parametric shape variation definition (see “Parametric shape variation,” Section 2.1.2). For the purposes of DSA if the parameter to which the shape variation data refer is a design parameter, the shape variation data are interpreted as the gradients of the nodal coordinates with respect to the design parameter. If a nonzero value is given for the shape parameter, Abaqus/Design will also perturb the base coordinates.
|
||
|
||
Input File Usage: Use the following option to specify the design gradients for shape design parameters:
|
||
|
||
\*PARAMETER SHAPE VARIATION, PARAMETER=design parameter
|
||
|
||
# Specifying gradients for non-shape design parameters
|
||
|
||
For non-shape design parameters, by default Abaqus/Design will use numerical differentiation to calculate design gradients based on the information you provide. However, you can override this default behavior by specifying the gradients directly using Python expressions (see “Parametric input,” Section 1.4.1). You specify a design parameter as the independent parameter and a list of the parameters that depend on that design parameter. Only one independent (design) parameter can be given for each design gradient definition.
|
||
|
||
Input File Usage: Use the following option to specify the design gradients for non-shape design parameters:
|
||
|
||
\*DESIGN GRADIENT, INDEPENDENT=design parameter, DEPENDENT=(list of dependent parameters)
|