김경종
353 lines
27 KiB
Markdown
353 lines
27 KiB
Markdown
<!-- source-page: 721 -->
|
||
|
||
Abaqus/CAE Usage: Use the following options to define translation and rotation of the substructure:
|
||
|
||
Assembly module: Instance→Translate or Instance→Rotate
|
||
|
||
Reflection of the substructure is not supported in Abaqus/CAE.
|
||
|
||
Use the following option to apply constraints that connect the retained nodes with the usage level nodes:
|
||
|
||
Interaction module: Constraint→Create
|
||
|
||
# Translating, rotating, and reflecting a substructure
|
||
|
||
Translation, rotation, and/or reflection (in that order) of a substructure can be specified in a substructure property definition.
|
||
|
||
Specify a translation by giving a translation vector. Specify a rotation by giving two points, a and b, defining a rotation axis plus a right-handed angular rotation around that axis. Specify a reflection by giving three non-colinear points in the reflection plane.
|
||
|
||
A translation does not affect the substructure’s stiffness or mass: the principal reason to apply a translation is to enable the tolerance check on nodal coordinates as discussed later. Rotation and/or reflection of a substructure affect the substructure’s stiffness and mass. The substructure load case definitions are rotated and/or reflected in the same way as the substructure’s stiffness and mass; therefore, all loads within substructure load cases are applied in the local directions associated with the substructure when it was created.
|
||
|
||
For distributed loads (for example, pressure loading of a surface) this application is precisely what is desired. However, distributed body forces in coordinate directions (BX, BY, BZ) are applied in the substructure’s local directions instead of in the global directions, which may not be what is needed. Similarly, distributed loadings that depend on position (for example, hydrostatic pressure or centrifugal loads) are based on the substructure’s local coordinates and not on the substructure position during usage. Be careful to ensure that loading of a rotated or shifted substructure is correct for its usage.
|
||
|
||
Whenever a substructure is translated, rotated, and/or reflected, the degrees of freedom at any retained nodes are with respect to the coordinate directions at the usage level. Therefore, if all of the degrees of freedom of a node are not retained or if a two-dimensional substructure is used in a three-dimensional model with rotation out of the x–y plane, additional degrees of freedom may be activated due to rotation and/or reflection. Be careful to check the validity of the substructure usage in such cases.
|
||
|
||
# Setting a tolerance on the substructure nodes
|
||
|
||
One difficulty with using large substructures is ensuring that the retained nodes in the substructure are connected to the correct nodes on the usage level (after substructure translation, rotation, and/or reflection, if applicable). Therefore, Abaqus/Standard checks that the coordinates of the retained nodes match the coordinates of the corresponding nodes on the usage level. A substructure does not require any coordinates on the usage level because it consists only of a stiffness matrix, a mass matrix, and a number of load cases. Nevertheless, it is usually a good check of a model’s validity to verify that the substructure and the model into which it is introduced are geometrically consistent.
|
||
|
||
<!-- source-page: 722 -->
|
||
|
||
To check the coordinates, you can set a tolerance on the distance between usage level nodes and the corresponding substructure nodes. This tolerance indicates the largest deviation allowable before a warning is issued. If you do not specify this tolerance, the default is to use a tolerance of $1 0 ^ { - 4 }$ times the largest overall dimension within the substructure. If you specify a tolerance of 0.0, the position of the retained nodes is not checked.
|
||
|
||
The geometric check is based on the coordinates of the retained nodes after translation, rotation, and/or reflection of the substructure at the usage level; motions of these nodes that occur as a result of geometrically nonlinear preloading during generation of the substructure are not considered in this check.
|
||
|
||
Input File Usage: \*SUBSTRUCTURE PROPERTY, ELSET=name, POSITION TOL=tolerance
|
||
|
||
Abaqus/CAE Usage: Assembly module: Instance→Translate and Instance→Rotate
|
||
|
||
# Defining substructure damping
|
||
|
||
Defining substructure damping at the substructure usage level means defining viscous and structural damping matrices for the finite elements associated with the substructures. Abaqus allows you to choose a particular source of damping for a substructure, to add several sources, or to exclude the damping effects for a substructure at the usage level. All options defining the substructure damping belong to a substructure property definition and affect only the finite elements of the substructure type associated with the substructure property.
|
||
|
||
# Sources of substructure damping
|
||
|
||
You can choose to model the damping of a substructure at the usage stage by using the reduced substructure damping matrices computed during the generation stage and stored on the substructure database. We denote the reduced viscous damping matrix of a substructure as $\overline { { C } } _ { r e d u c e d }$ and the reduced structural damping matrix of a substructure as $\overline { { S } } _ { r e d u c e d }$ . Alternatively, you can introduce the stiffness and mass proportional damping matrices by multiplying the reduced substructure stiffness and mass matrices, $\bar { \overline { { K } } } _ { r e d u c e d }$ and $\bar { M } _ { r e d u c e d }$ , respectively, with the factors defined within the substructure property definition at the usage stage. You can also combine both damping sources or exclude the effects of damping altogether at the usage level. Finally, you can introduce viscous and structural modal damping matrices for a substructure specifying damping coefficients for the substructure eigenmodes calculated at the generation stage and stored on the substructure database.
|
||
|
||
The substructure modal damping contributes to the damping matrices for the finite elements associated with a substructure, and it can be used instead of or together with the other substructure damping sources. To define the substructure modal damping matrix, you specify the diagonal damping matrix on the substructure modal subspace. This matrix is transformed to the substructure degrees of freedom space to be added to the damping matrix of the finite element associated with the substructure.
|
||
|
||
# Controlling the sources of substructure viscous damping
|
||
|
||
In the general case the substructure type element viscous damping matrix at the usage stage is defined by the following matrix equation:
|
||
|
||
$$
|
||
\overline {{C}} = \overline {{C}} _ {r e d u c e d} + \alpha \overline {{M}} + \beta \overline {{K}} + \overline {{C}} _ {m o d a l}.
|
||
$$
|
||
|
||
<!-- source-page: 723 -->
|
||
|
||
You can specify substructure viscous damping using substructure damping controls and/or substructure viscous modal damping. If you specify substructure viscous modal damping, it is used in combination with all other activated viscous damping sources to form the viscous damping matrix of the finite element. Defining the substructure viscous modal damping is discussed in more detail in “Defining substructure viscous modal damping” below.
|
||
|
||
# Input File Usage:
|
||
|
||
To activate only the generated condensed viscous damping matrix of the substructure (the first term on the right-hand side), use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=ELEMENT
|
||
|
||
To activate only the stiffness and mass proportional substructure viscous damping, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=FACTOR
|
||
|
||
To activate the combined generated and proportional substructure viscous damping matrix, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=COMBINED
|
||
|
||
To exclude the effects of generated and proportional substructure viscous damping altogether at the usage level, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, VISCOUS=NONE
|
||
|
||
To specify the substructure viscous modal damping matrix (the last term on the right-hand side), use the following option:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING
|
||
|
||
# Abaqus/CAE Usage:
|
||
|
||
Substructure damping controls and substructure modal damping are not supported in Abaqus/CAE.
|
||
|
||
# Controlling the sources of substructure structural damping
|
||
|
||
In the general case the substructure type element structural damping matrix is defined by the following equation:
|
||
|
||
$$
|
||
\overline {{S}} = \overline {{S}} _ {r e d u c e d} + \gamma \overline {{K}} _ {r e d u c e d} + \overline {{S}} _ {m o d a l}.
|
||
$$
|
||
|
||
You can specify substructure structural damping using substructure damping controls and/or substructure structural modal damping. If you specify substructure structural modal damping, it is used in combination with all other activated structural damping sources to form the structural damping matrix of the finite element. Defining the substructure structural modal damping is discussed in more detail in “Defining substructure structural modal damping” below.
|
||
|
||
# Input File Usage:
|
||
|
||
To activate only the generated reduced structural damping matrix of the substructure (the first term on the right-hand side), use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=ELEMENT
|
||
|
||
<!-- source-page: 724 -->
|
||
|
||
To activate only the stiffness proportional substructure structural damping matrix, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=FACTOR
|
||
|
||
To activate the combined generated and stiffness proportional structural damping matrix, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=COMBINED
|
||
|
||
To exclude the generated and stiffness proportional structural damping matrices, use the following option:
|
||
|
||
\*SUBSTRUCTURE DAMPING CONTROLS, STRUCTURAL=NONE
|
||
|
||
To specify the substructure structural modal damping matrix (the last term on the right-hand side), use the following option:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING
|
||
|
||
Abaqus/CAE Usage: Substructure damping controls and substructure modal damping are not supported in Abaqus/CAE.
|
||
|
||
# Defining substructure damping factors
|
||
|
||
By default, the damping factors, and , and the structural damping factor, , used to define stiffness proportional and mass proportional damping for a substructure are zeros.
|
||
|
||
Input File Usage: Use the following options to define the values of the substructure damping factors at the usage level:
|
||
|
||
\*SUBSTRUCTURE DAMPING, ALPHA= , BETA= , STRUCTURAL=
|
||
|
||
Abaqus/CAE Usage: Defining substructure damping factors is not supported in Abaqus/CAE.
|
||
|
||
# Defining substructure viscous modal damping
|
||
|
||
Substructure viscous modal damping is defined for the substructure eigenmodes extracted at the substructure generation level. The mode numbers and the eigenfrequencies used to define substructure viscous modal damping come from the solution of the substructure eigenvalue problem at the generation level.
|
||
|
||
Input File Usage: Use the following option to define the fraction of critical damping for a substructure by specifying mode numbers:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=MODE NUMBERS
|
||
|
||
Use the following option to define the fraction of critical damping for a substructure by specifying a frequency range:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, DEFINITION=FREQUENCY RANGE
|
||
|
||
<!-- source-page: 725 -->
|
||
|
||
Use the following option to define substructure modal Rayleigh damping by specifying the substructure mode numbers:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=MODE NUMBERS
|
||
|
||
Use the following option to define substructure modal Rayleigh damping by specifying a frequency range:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=FREQUENCY RANGE
|
||
|
||
Abaqus/CAE Usage: Substructure modal damping is not supported in Abaqus/CAE.
|
||
|
||
Defining substructure structural modal damping
|
||
|
||
Substructure structural modal damping is defined for the substructure eigenmodes extracted at the substructure generation level. The mode numbers and the eigenfrequencies used to define substructure structural modal damping come from the solution of the substructure eigenvalue problem at the generation level.
|
||
|
||
Input File Usage: Use the following option to define substructure structural modal damping by specifying mode numbers:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS
|
||
|
||
Use the following option to define substructure structural modal damping by specifying a frequency range:
|
||
|
||
\*SUBSTRUCTURE MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE
|
||
|
||
Abaqus/CAE Usage: Substructure modal damping is not supported in Abaqus/CAE.
|
||
|
||
# Defining kinematic constraints and transformations
|
||
|
||
All kinematic boundary conditions, MPCs, and transformations can be applied to retained degrees of freedom at the usage level. These specifications can be changed from step to step in the usual way. In this respect substructures and their retained nodes act in an identical manner to regular elements and their nodes.
|
||
|
||
# Defining transformations at retained nodes
|
||
|
||
If a nodal transformation (“Transformed coordinate systems,” Section 2.1.5) is used during substructure generation at a retained node, the transformations are built into the substructure. This creates an inconsistency when the substructure node is attached to a standard Abaqus element since Abaqus/Standard uses the retained degrees of freedom directly without checking their directions. Therefore, it is suggested that this situation be avoided.
|
||
|
||
If a nodal transformation must be used, the resulting inconsistency can be resolved by retaining all degrees of freedom at the node and applying a linear constraint equation (“Linear constraint equations,”
|
||
|
||
<!-- source-page: 726 -->
|
||
|
||
Section 35.2.1) as follows. At any point where such a transformed substructure node is attached to a global model, define two coincident nodes on the usage level, P and Q, for example. Use node P for the substructure at the usage level (defined with an element definition); the local directions of the degrees of freedom are already built in at this node. Use node Q for all standard Abaqus elements attached to this point. Use a local transformation at node Q to transform the degrees of freedom to the same local directions that are built-in for node P. Now use a linear constraint equation to equate the individual degrees of freedom at nodes P and Q.
|
||
|
||
# Applying loads to a substructure
|
||
|
||
Loads or boundary conditions that are to be applied to a substructure within an analysis (at the usage level) must be specified during the substructure generation step by defining a substructure load case or by requesting that the substructure’s gravity load vectors be calculated (see “Defining substructure load cases for subsequent loading in an analysis” in “Defining substructures,” Section 10.1.2). A load case can be made up of any combination of loadings and nonzero boundary conditions, and multiple load cases can be defined for any given substructure.
|
||
|
||
When you activate load cases created for a substructure, you specify the element number or element set name of the substructures, the associated substructure load case names, and the scaling multipliers for the specified substructure load case loads and/or boundary conditions. To reproduce the loading conditions defined during substructure generation exactly, use a magnitude of 1.0.
|
||
|
||
Boundary conditions specified during a substructure’s generation are always present, whether the substructure load case that they are part of is active or not. They are effectively built into the substructure and can only be scaled if desired but not removed. See “Defining substructures,” Section 10.1.2, for further information about defining boundary conditions in substructures.
|
||
|
||
Input File Usage: Use the following option to activate a substructure load case: \*SLOAD
|
||
|
||
Abaqus/CAE Usage: Use the following option to activate a substructure load case:
|
||
|
||
Load module: load editor: Category: Mechanical: Types for Selected Step: Substructure load
|
||
|
||
# Modifying or removing load cases
|
||
|
||
By default, substructure loads are applied as modifications of existing loads or in addition to any loads previously defined. You can remove all previously defined loads and, optionally, specify new loads when you activate a load case. Boundary conditions cannot be removed.
|
||
|
||
Input File Usage: Use the following option to modify load cases:
|
||
|
||
\*SLOAD, OP=MOD
|
||
|
||
Use the following option to remove load cases:
|
||
|
||
\*SLOAD, OP=NEW
|
||
|
||
Abaqus/CAE Usage: Use the following option to modify load cases:
|
||
|
||
Load module: Load Case Manager: click Edit
|
||
|
||
<!-- source-page: 727 -->
|
||
|
||
Use the following option to remove load cases:
|
||
|
||
Load module: Load Case Manager: click Delete
|
||
|
||
# Specifying time-dependent load cases
|
||
|
||
The magnitude of substructure loads can be varied with time by referring to an amplitude definition (“Amplitude curves,” Section 34.1.2).
|
||
|
||
Input File Usage: Use the following options to define time-dependent load cases:
|
||
|
||
\*AMPLITUDE, NAME=amplitude \*SLOAD, AMPLITUDE=amplitude
|
||
|
||
Abaqus/CAE Usage: Use the following options to define time-dependent load cases:
|
||
|
||
Load module: amplitude editor: Create Amplitude: Amplitude: amplitude
|
||
|
||
Load module: load editor: Category: Mechanical: Types for Selected
|
||
|
||
Step: Substructure load: Amplitude: amplitude
|
||
|
||
# Load cases in geometrically nonlinear analyses
|
||
|
||
All substructure loads and boundary conditions are applied in a local system associated with the substructure. Since this local system rotates with the substructure when large motions are present, these loads and boundary conditions will rotate as well. As a consequence, you should be careful when using substructure loads in geometrically nonlinear analyses to ensure that the loading is in the appropriate direction at the usage level. This situation is similar to rotating the substructure via a substructure property definition.
|
||
|
||
# Gravity loading
|
||
|
||
A distributed load definition can be used to apply gravity loading to a substructure with a user-defined magnitude, scaled by an amplitude definition, and acting in a specifed direction. To enable gravity loading for a substructure, you must request the calculation of the substructure’s gravity load vectors during the substructure generation step (see “Gravity loading” in “Defining substructures,” Section 10.1.2). In this case gravity loading should not be defined as part of a substructure load case.
|
||
|
||
Input File Usage: Use the following option to define gravity loading:
|
||
|
||
\*DLOAD, AMPLITUDE=amplitude element set or element number, GRAV, magnitude, direction
|
||
|
||
Abaqus/CAE Usage: Load module: Create Load: choose Mechanical for the Category and Gravity for the Types for Selected Step
|
||
|
||
# Obtaining output of results within a substructure
|
||
|
||
You can obtain output within substructures used in static, dynamic, eigenfrequency extraction, and steady-state and transient modal dynamic analyses. The recovery of output is not possible for substructures used in response spectrum and random response analyses. Output within a substructure
|
||
|
||
<!-- source-page: 728 -->
|
||
|
||
does not include the displacements, stresses, etc. resulting from the preload deformation of a substructure.
|
||
|
||
Output within substructures is available in the data (.dat) file, in the results (.fil) file, and in output database (.odb) files. Separate output database files are created for each substructure using the naming convention inputfile-name\_substructure-number.odb. If a substructure contains a nested substructure, a file called inputfile-name\_substructure-number\_nested-substructure-number.odb is created containing the output for the nested substructure. The abaqus substructurecombine execution procedure can combine model and results data from two substructure output databases into a single output database. For more information, see “Combining output from substructures,” Section 3.2.24.
|
||
|
||
Recovery of the solution within substructures requires that the information for recovering the data within a substructure be available from the .sup, .sim, .prt, .stt, and .mdl files.
|
||
|
||
Output is organized substructure by substructure: you direct Abaqus/Standard to go inside a particular substructure and then request output for that substructure. Results can be recovered within nested multilevel substructures only if the substructure libraries for all substructures in the chain are available.
|
||
|
||
Substructure output requests are most easily pictured by thinking of substructures as “levels” of detailed modeling. At the global (top) level we have the analysis model (for example, an airplane). Dropping down from this level to the first substructure level, we have the main components of the model defined as substructures (wings, stabilizer, fuselage, etc.). Dropping down to the second substructure level, we have other substructures (flaps, tanks, floors, etc.), which, in turn, may contain third level substructures (spars, stringers, etc.), and so on. To obtain output, you move down and back up through these various levels using substructure paths, similar to the way you navigate a tree structure for file directories. Each substructure path definition consists of entering into a substructure at the next level down or leaving the current substructure and moving up one level in the tree.
|
||
|
||
At the start of the output requests, Abaqus/Standard is at the global model level. You must always enter and leave a substructure consistently, so that after a set of substructure output requests Abaqus/Standard is left at the global model level. You must return to the global level (outside all substructures) before the end of the step definition.
|
||
|
||
If you enter and leave in the same substructure path definition, the effect is to leave the substructure and enter another substructure at the same level.
|
||
|
||
# Entering a substructure for output
|
||
|
||
To enter a particular substructure for output, you identify the substructure by the element number n chosen for it in the model. All subsequent output requests are for output within that substructure and must be given in terms of its internal node and element numbers (the node and element numbers used when the substructure was created).
|
||
|
||
Input File Usage: \*SUBSTRUCTURE PATH, ENTER ELEMENT=n
|
||
|
||
Abaqus/CAE Usage: Step module: field output request editor: Domain: Substructure: click the Edit button, and select substructure sets
|
||
|
||
<!-- source-page: 729 -->
|
||
|
||
# Leaving a substructure after obtaining output
|
||
|
||
After you have obtained output for a substructure, you must return to the level of the model of which the substructure forms a part, thus indicating the end of the output requests for variables within that substructure.
|
||
|
||
Input File Usage: \*SUBSTRUCTURE PATH, LEAVE
|
||
|
||
Abaqus/CAE Usage: Step module: field output request editor: Domain: Substructure: click the Edit button, and select substructure sets
|
||
|
||
# Obtaining output if substructures are nested
|
||
|
||
You must enter several substructures if substructures are used at multiple levels and output is required several levels down. Nesting of substructures is not supported in Abaqus/CAE.
|
||
|
||
# Example: obtaining output within nested substructures
|
||
|
||
For example, suppose that a model includes several substructures at two levels. Printed output of stress components is required in some elements within two substructures at the second level, as well as printed output of the displacements at some of the nodes of one of the first-level substructures. (Recall that “first-level” refers to substructures used directly in the analysis model; “second-level” substructures are used as components of first-level substructures.)
|
||
|
||
The data might be as follows:
|
||
|
||
```txt
|
||
*SUBSTRUCTURE PATH, ENTER ELEMENT=N
|
||
** This option takes us into element number N, which must be a substructure.
|
||
*SUBSTRUCTURE PATH, ENTER ELEMENT=M
|
||
** We now drop down into element number M of this substructure.
|
||
** M is the element number used for this substructure when N was created.
|
||
** M must refer to a substructure.*EL PRINT, ELSET=A1
|
||
S
|
||
** This option requests stress output in element set A1 of this substructure.
|
||
** This element set must have been defined during the creation of substructure M.
|
||
*SUBSTRUCTURE PATH, LEAVE
|
||
** This option takes us back up into first-level substructure N.
|
||
*SUBSTRUCTURE PATH, ENTER ELEMENT=P
|
||
** This option takes us down into element P, which must again be a substructure in element N.
|
||
*EL PRINT, ELSET=A1
|
||
S
|
||
** This option requests the printing of stress output in element set A1. It is possible that
|
||
** this is the same set of elements in the same substructure as was used in the request above
|
||
** because substructures M and P may both be copies of the same substructure.
|
||
** However, the stresses will presumably be different because they represent the same
|
||
** component in different locations in the model.
|
||
```
|
||
|
||
<!-- source-page: 730 -->
|
||
|
||
*SUBSTRUCTURE PATH, LEAVE
|
||
** Back to N.
|
||
*SUBSTRUCTURE PATH, LEAVE
|
||
** We are now back at the global level.
|
||
*SUBSTRUCTURE PATH, ENTER ELEMENT=R
|
||
** Enter element R at the global level: this element is the substructure in which we want
|
||
** to print the displacements.
|
||
*NODE PRINT, NSET=FLANGE
|
||
U
|
||
** This option prints the displacements at all nodes in node set
|
||
** FLANGE of the substructure.
|
||
** Again, FLANGE must have been defined when the substructure was
|
||
** created.
|
||
*SUBSTRUCTURE PATH, LEAVE
|
||
** Back to the global level.
|
||
|
||
# Interpreting nodal variable output
|
||
|
||
The nodal displacements within the substructure do not include the displacements resulting from the preload deformation if it exists.
|
||
|
||
If a substructure is rotated and/or reflected, nodal variables are output relative to the global coordinate system of the analysis. In a geometrically nonlinear analysis, the nodal displacements will include the large motions associated with the translation and rotation of the substructure in addition to the small-strain displacements. If a nodal transformation (“Transformed coordinate systems,” Section 2.1.5) has been used, nodal output will be in either the local or the global directions, depending on the nodal output request (see “Output to the data and results files,” Section 4.1.2). If a nodal transformation has been used during substructure generation, the transformed directions are rotated with the substructure.
|
||
|
||
# Interpreting element variable output
|
||
|
||
Element output variables within a substructure do not include the values of the variable resulting from the preload deformation if it exists.
|
||
|
||
Element variables in continuum elements are output relative to the global coordinate system of the analysis model or in the local (material) coordinate system if one has been used (“Orientations,” Section 2.2.5). Element output for structural elements is always given with respect to the element coordinate system used during substructure generation. Integration point coordinates and local material directions (see “Output to the data and results files,” Section 4.1.2) are given with respect to the global coordinate system.
|
||
|
||
Element quantities associated with nonlinear preload response (plastic strains, creep strains, etc.) can be output during a substructure recovery. Since the response in a substructure during its usage is entirely linear, these quantities, which are part of the base state, do not change from the values computed during the preload.
|