김경종
21 KiB
If a substructure was reflected, the element connectivities of continuum elements written to the substructure instance output database are adjusted so as not to violate the Abaqus convention for counterclockwise element numbering.
You cannot directly obtain the element output for the element centroidal values or the element output at the element nodes when you recover results within substructures. This output data can be calculated from the substructure-related data in the output database file using commands in the Abaqus Scripting Interface.
Interpreting results written to the results file
Results within substructures can be written to the results file. Substructure path records are inserted in the results file to indicate the switch into a substructure: all records following such a record belong to the substructure defined on that record until the next substructure path record appears in the file.
Requests for output to the results file will cause Abaqus/Standard to write the definitions of elements and nodes at the global level and within all substructures in the model to the file. As with the results records themselves, these records for nodes and elements within substructures will be preceded and followed by substructure path records to indicate that they belong to that substructure.
Node and element numbers within each substructure are local to that substructure, so that the same node and element numbers may appear in several substructures and in the global level model. In such a case the substructure path records must be used to identify the location of a particular node or element within the model. If you can ensure that node and element numbers are unique throughout the entire model, including all substructures, the substructure path records in the results file can be ignored.
Visualizing substructure results
While Abaqus/CAE does not support substructures directly, you can view substructure results by combining all of the substructure instance output database (.odb) files into a single file. See “Combining output from substructures,” Section 3.2.24, for details.
You can also load and view each individual substructure instance output database (.odb) file separately in Abaqus/CAE.
Substructure library compatibility
A substructure usage analysis can use the substructure libraries generated from the same or any previous maintenance delivery of the same general release. The substructure library is not compatible between general releases.
A substructure usage analysis must be run on a computer that is binary compatible with the computer used to generate the substructure library.
Input file template
The following template can be used to generate a substructure:
*HEADING
...
*NODE, NSET=N1
Data lines to define the nodes.
*NSET,NSET=N3
Data lines to define the node set members.
*ELEMENT, TYPE=CPE8, ELSET=E1
Data lines to define the elements that make up the substructure.
*ELSET,ELSET=E3
Data lines to define the element set members.
*SOLID SECTION, ELSET=E1, MATERIAL=M1
*MATERIAL, NAME=M1
*ELASTIC
30.E6, 0.3
*DENSITY
0.0007324
*STEP
*FREQUENCY
Data line to specify the number of modes ( m). The *FREQUENCY option is required if modes are requested using the *SELECT EIGENMODES option.
*END STEP
*STEP
*STATIC
Options to define a linear or nonlinear static preload.
*END STEP
*STEP
*SUBSTRUCTURE GENERATE, TYPE=Z101, OVERWRITE, MASS MATRIX=YES,VISCOUS DAMPING MATRIX=YES, STRUCTURAL DAMPING MATRIX=YES,RECOVERY MATRIX=YES, NSET=N3, ELSET=E3
*RETAINED NODAL DOFS
Data lines to define the retained degrees of freedom.
*SELECT EIGENMODES, GENERATE
1, m, 1
*SUBSTRUCTURE LOAD CASE, NAME=LOADS
*CLOAD
Data lines to define concentrated loading.
*DLOAD
Data lines to define distributed loading.
*END STEP
The following template can be used to define substructure instances:
*HEADING
...
*ELEMENT, TYPE=Z101, ELSET=E2
Data line to define the element.
*SUBSTRUCTURE PROPERTY, ELSET=E2
*BOUNDARY
...
*RESTART, WRITE
*STEP
*STATIC
...
*BOUNDARY
...
*SLOAD
E2, LOADS, scale factor
*SUBSTRUCTURE PATH, ENTER ELEMENT=n
*EL PRINT
S,
*NODE PRINT
U,
*SUBSTRUCTURE PATH, LEAVE
*END STEP
*STEP
*DYNAMIC
...
*BOUNDARY
...
*SUBSTRUCTURE PATH, ENTER ELEMENT=n
*EL PRINT
S,
*NODE PRINT
U, V
*SUBSTRUCTURE PATH, LEAVE
*END STEP
10.1.2 DEFINING SUBSTRUCTURES
Products: Abaqus/Standard Abaqus/CAE
References
• “Using substructures,” Section 10.1.1
• *RETAINED NODAL DOFS
• *SELECT EIGENMODES
• *SUBSTRUCTURE COPY
• *SUBSTRUCTURE DELETE
• *SUBSTRUCTURE DIRECTORY
• *SUBSTRUCTURE GENERATE
• *SUBSTRUCTURE LOAD CASE
• *SUBSTRUCTURE MATRIX OUTPUT
• *MATRIX CHECK
• *FLEXIBLE BODY
Overview
This section describes how individual substructures are defined. See “Using substructures,” Section 10.1.1, for information regarding how they are used in a model.
Substructures are defined using the substructure generation procedure. The substructure creation and usage cannot be included in the same analysis. Multiple substructures can be generated in an analysis. Any substructure can consist of one or more other substructures; if this is the case, the nested-level substructures must be defined first. The substructure library is not organized in terms of part instances; therefore, substructures cannot be generated from models that have an assembly defined. None of the substructure options are supported in models that have an assembly defined.
To define a typical substructure generation step, do the following:
• Invoke the substructure generation procedure.
• Define the nodes and degrees of freedom that are to be retained as external degrees of freedom when the substructure is used.
• Optionally, retain extra dynamic modes to improve the dynamic behavior of the substructure during usage.
• Optionally, specify substructure load cases.
• Optionally, write the recovery matrix, substructure’s stiffness matrix, mass matrix, and/or load case vectors to a file.
Generating a substructure
When you generate a substructure, you specify an identifier that will be assigned to this substructure in a substructure library. The identifier must begin with the letter Z followed by a number that cannot exceed 9999.
Substructure identifiers must be unique within a library. If a substructure with this same identifier already exists in the library, the analysis will terminate with an error message unless you have specified that the existing substructure should be overwritten, as described below.
Input File Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Substructure generation: n
Substructure database
A substructure database is the set of files that describe the geometry of a substructure, and Abaqus writes all substructure data to the substructure database during the analysis. The substructure database can include files with the following extensions: .sup, .sim, .prt, .mdl, and .stt; the .sup file is called the substructure library. By default, substructure data are written to a substructure database named jobname, and the substructure files are named jobname.sup, jobname_Zn.sim, jobname_Zn.prt, jobname_Zn.mdl, and jobname_Zn.stt. Files with the extensions .sup and .sim are generated for all substructures. Files with the extensions .prt, .mdl, and .stt are generated only if the solution within the substructure can be fully or partially recovered. Several substructures can share a substructure library file, but other files are individual for each substructure. It is strongly recommended that the substructure library name be different for different substructures.
You can choose to write the data to a user-specified substructure database.
If you specify the substructure library name, the files will be named library_name_Zn.sim, library_name_Zn.prt, library_name_Zn.mdl, and library_name_Zn.stt.
Input File Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name
Abaqus/CAE Usage: Definition of substructure libraries is not supported in Abaqus/CAE.
Overwriting the substructure data in a library
If a substructure generation analysis is rerun using the same jobname without deleting the substructure library and one substructure or more will be regenerated, you must specify that the existing substructures can be overwritten. This requirement also holds true if the jobname is different for the second analysis but the same library_name is specified.
Input File Usage: *SUBSTRUCTURE GENERATE, TYPE=Zn, LIBRARY=library_name, OVERWRITE
Abaqus/CAE Usage: Definition of substructure libraries is not supported in Abaqus/CAE.
Recovery within a substructure
By default, the solution at any degree of freedom in the substructure can be recovered. Abaqus must have access to the substructure’s .mdl, .prt, and .stt files to perform a full recovery. These files all reside in the substructure database.
You can specify that a recovery of element or nodal information will not be required within this substructure. This reduces the size of the substructure database significantly for a large substructure because the information that is needed to recover eliminated variables is not stored. However, this information cannot be recreated at a later time except by regenerating the entire substructure with recovery enabled.
Input File Usage: Use the following option to enable recovery for a substructure:
*SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=YES (default)
Use the following option to disable recovery for a substructure:
*SUBSTRUCTURE GENERATE, TYPE=Zn, RECOVERY MATRIX=NO
Abaqus/CAE Usage: Use the following option to enable recovery for a substructure:
Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Whole model
Use the following option to disable recovery for a substructure:
Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle off Evaluate recovery matrix for
Using the selective recovery method
If results recovery is desired only at a subset of the internal degrees of freedom, disk usage can be reduced substantially by using the selective recovery method. To enable selective recovery, the region where recovery is desired can be specified directly.
Input File Usage: Use the following option to define the node set for selective recovery:
*SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, NSET=Node set name
Use the following option to define the element set for selective recovery:
*SUBSTRUCTURE GENERATE, RECOVERY MATRIX=YES, ELSET=Element set name
Abaqus/CAE Usage: Use the following option to define the node set for selective recovery:
Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Node set name
Use the following option to define the element set for selective recovery:
Step module: Create Step: Linear perturbation: Substructure generation: Basic tabbed page: toggle on Evaluate recovery matrix for: select Region: Element set name
Evaluating frequency-dependent material properties
When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in substructure generation. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness at zero frequency and does not consider the stiffness contributions from frequency-domain viscoelasticity. If you do specify a frequency, only the real part of the stiffness contributions from frequency-domain viscoelasticity is considered.
Input File Usage: *SUBSTRUCTURE GENERATE, PROPERTY EVALUATION=frequency
Abaqus/CAE Usage: Step module: Step editor: Substructure generate: Options tabbed page: toggle on Evaluate frequency-dependent properties at frequency: frequency
Defining the retained degrees of freedom
The degrees of freedom at a node can be divided into retained degrees of freedom (for use at the usage level of the substructure) and eliminated degrees of freedom (internal to the substructure). Abaqus/Standard allows any of the degrees of freedom at any of the nodes of a substructure to be retained with one exception: if an acoustic-structural substructure is generated, based on coupled or uncoupled modes, only structural degrees of freedom can be retained. You must make sure that the choice of retained degrees of freedom is reasonable so that the substructure can be connected correctly to the rest of the model.
Any degrees of freedom where kinematic constraints may have to be respecified during usage of the substructure should be kept as retained degrees of freedom.
If any degrees of freedom of nodes used to define distributing coupling elements are retained, the degrees of freedom of an internal node associated with the Lagrange multipliers are added automatically to the list of the retained degrees of freedom of the substructure.
To define the retained degrees of freedom, specify the node number or node set label and, optionally, the first and the last degree of freedom to be retained.
By default, the nodes associated with the retained degrees of freedom will be sorted into ascending numerical order.
Input File Usage: *RETAINED NODAL DOFS
Abaqus/CAE Usage: Load module: boundary condition editor: Category: Mechanical: Types for Selected Step: Retained nodal dofs
Preventing the degrees of freedom from being sorted
You can prevent the degrees of freedom from being sorted. The ordering of the nodes when using a substructure is then the same as the ordering used when specifying the retained nodes.
Input File Usage: *RETAINED NODAL DOFS, SORTED=NO
Abaqus/CAE Usage: You cannot prevent retained nodes from being sorted in Abaqus/CAE.
Retaining degrees of freedom when the substructure is intended for geometrically nonlinear analysis at the usage level
When the substructure is intended for use in geometrically nonlinear analyses, it is recommended to retain all translational and/or all rotational degrees of freedom from a particular node. Even in the case when only a single translational/rotational degree of freedom of a particular node is deemed as needed at the usage level, you should retain all translational/rotational degrees of freedom associated with that node. Otherwise, as the substructure rotates during a geometrically nonlinear analysis, local numerical instabilities (negative eigenvalues) may occur since the rotated substructure may have no stiffness in particular degrees of freedom.
You must choose an appropriate number of nodes that will allow for the computation of an equivalent rigid body motion of the substructure. In two-dimensional or axisymmetric analyses, retaining two nodes with all translational degrees of freedom or one node with all translational and rotational degrees of freedom is sufficient to compute an equivalent rigid body motion of the substructure at the usage level. In three-dimensional analysis, three non-colinear nodes with all translational degrees of freedom retained or one node with all translations and rotations are needed. If the retained nodes are colinear or fewer than three nodes are retained, you must retain at least one node with all rotational degrees of freedom. When Abaqus/Standard cannot compute an equivalent rigid body motion for the substructure during the analysis at the usage level because the number of retained degrees of freedom is not appropriate, a warning message is issued and any geometrically nonlinear effects associated with the substructure are ignored.
Defining kinematic constraints
Kinematic constraints are defined as described in “Kinematic constraints: overview,” Section 35.1.1. The following rules apply:
• All kinematic boundary conditions associated with degrees of freedom that are not retained must be specified when the substructure is generated. The conditions are built into the substructure and remain imposed any time that it is used. Once the substructure is generated, kinematic constraints on internal variables cannot be respecified; they can be modified or removed only by erasing and recreating the substructure in the library. The magnitude of a prescribed boundary condition applied to an internal degree of freedom can be associated with a substructure load case and can be changed at the usage level. The restraint itself is built into the substructure and cannot be removed by omitting a reference to the load case.
• During substructure generation, multi-point constraints in which some of the substructure’s retained degrees of freedom are eliminated in favor of internal degrees of freedom must be avoided. If it
is desirable to retain certain degrees of freedom that are eliminated by the multi-point constraints, you must reassign all of the variables appearing in the multi-point constraints as retained degrees of freedom and impose the constraints at the usage level.
Defining the generalized degrees of freedom
An effective technique for modeling the dynamic behavior of a substructure is to augment the response within the substructure by including some generalized degrees of freedom associated with the dynamic modes. You can select the modes to retain, which must be calculated in a previous frequency extraction step (“Natural frequency extraction,” Section 6.3.5). For some cases of the substructure generation, the dynamic modes have to be fully recovered; if they were computed with the AMS eigensolver and only partially recovered, an error message is issued in such cases. For example, if a substructure includes the substructure load cases or structural-acoustic coupling (or it will be used for flexible body generation) the eigenmodes have to be fully recovered. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. If all retained degrees of freedom of the substructure are constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Bampton method. If all retained degrees of freedom of the substructure are not constrained in the frequency extraction step, this technique is commonly referred to as the Craig-Chang method. The substructure dynamic modes in the Craig-Bampton method are commonly referred to as the fixed-interface modes, and the substructure dynamic modes in the Craig-Chang method are commonly referred to as the freeinterface modes. If some retained degrees of freedom of the substructure are constrained and other retained degrees of freedom are not constrained in the frequency extraction step, the dynamic modes are called mixed-interface modes. If the free-interface or mixed-interface dynamic modes are selected, the substructure generation time can increase substantially compared to the case when the same number of fixed-interface dynamic modes is used. Abaqus issues a warning message in this case. However, better solution accuracy can sometimes be achieved with a significantly smaller number of free- or mixed-interface dynamic modes than by using fixed-interface modes.
A sufficient number of the dynamic modes should be selected to provide adequate dynamic representation of the substructure. You should examine loading frequencies and frequency content of the structure to determine this range. Specify a shift point and/or a cutoff frequency in the eigenfrequency extraction step definition to obtain modes in the desired frequency range only. Inclusion of generalized degrees of freedom adds the cost of the frequency extraction to the substructure generation step but greatly improves the accuracy of the solution if the substructure is used in a subsequent dynamic (“Implicit dynamic analysis using direct integration,” Section 6.3.2), steady-state dynamic (“Direct-solution steady-state dynamic analysis,” Section 6.3.4), or frequency extraction (“Natural frequency extraction,” Section 6.3.5) analysis.
In the case of the displacement normalization of the eigenvectors in a frequency extraction analysis, a substructure must have at least one physical degree of freedom active on the usage level; otherwise, the modes cannot be normalized properly. See “Substructuring and substructure analysis,” Section 2.14.1 of the Abaqus Theory Guide, for additional details.
The retained eigenmodes must be selected when an acoustic-structural substructure is generated.
The effect of acoustic-structural coupling can be included in the retained eigenmodes during the natural frequency extraction procedure. To calculate the coupled structural-acoustic eigenmodes, use a