OVERVIEW OF SUBSTRUCTURES IN Abaqus/CAE39.SubstructuresThis section explains how to integrate substructures into your analysis in Abaqus/CAE.The following topics are covered:•“Overview of substructures in Abaqus/CAE,”Section39.1•“Generating a substructure,”Section39.2•“Specifying the retained nodal degrees of freedom and load cases for a substructure,”Section39.3•“Importing a substructure into Abaqus/CAE,”Section39.4•“Using substructure part instances in an assembly,”Section39.5•“Recoveringfield output for substructures,”Section39.7•“Visualizing substructure output,”Section39.839.1Overview of substructures in Abaqus/CAESubstructures are collections of elements that have been grouped together,so the internal degrees of freedom have been eliminated for the ing a substructure make model definition easier and analysis faster when you analyze a model that contains identical pieces that appear multiple times(such as the teeth of a gear),because you can use a substructure repeatedly in a model.Substructures are connected to the rest of the model by the retained degrees of freedom at the retained nodes.Factors that determine how many and which nodes and degrees of freedom should be retained are discussed in “Defining substructures,”Section10.1.2of the Abaqus Analysis User’s Manual.Substructure definition in your model follows two sets of steps:•“Creating substructures in your model database,”Section39.1.1•“Including substructures in your analysis,”Section39.1.239.1.1Creating substructures in your model databaseYou can create substructures in Abaqus/CAE by following these general steps:1.Create or open the model database in which you want to specify substructures in Abaqus/CAE.2.In the Step module,create a Substructure generation step.Abaqus/CAE converts the entiremodel into a single substructure.For more information,see“Generating a substructure,”Section39.2.3.In the Load module,create Retained nodal dofs boundary conditions to determine which degreesof freedom will be retained as external degrees of freedom on the substructure.You can also definea load case in the substructure generation step if you want to apply a load to the substructure atGENERA TING A SUBSTRUCTUREa location other than its retained degrees of freedom.For more information,see“Specifying theretained nodal degrees of freedom and load cases for a substructure,”Section39.3.4.In the Job module,create a new job and submit the analysis.When you perform an analysis of an assembly that includes substructure data,Abaqus/CAE creates separate output databases for the results of each substructure part instance and does not include the results from the substructure part instances in the output database for the assembly.The Visualization module provides tools that enable you to integrate the results from the substructure components back into the results from the assembly;for more information,see“Visualizing substructure output,”Section39.8.39.1.2Including substructures in your analysisSubstructure usage should be performed in a different model than substructure generation.You can include substructures in your analysis in Abaqus/CAE by following these general steps:1.Import each substructure that you want to use in your model database from the corresponding.simfile.For more information,see“Importing a substructure into Abaqus/CAE,”Section39.4,in the online HTML version of this manual.2.In the Assembly module,instance each substructure part that you want to add to the assembly,andposition the substructure part instances in the desired locations in the assembly.“Using substructure part instances in an assembly,”Section39.5,explains the capabilities and limitations of substructure part instances.3.In the Load module,activate substructure load cases by creating a Substructure load definition.For more information,see“Activating load cases during substructure usage,”Section39.6.4.In the Step module,create afield output request with Substructure as the Domain,then select thesubstructure sets for which you want to recoverfield data.For more information,see“Recovering field output for substructures,”Section39.7.5.In the Interaction module,apply constraints to attach the substructure part instance to the rest of theassembly.39.2Generating a substructureThefirst step in substructure definition is the addition of a Substructure generate step in your analysis.The substructure generation step enables you to create a substructure in your model database and,if desired,specify substructure-related options such as the writing of the recovery matrix,stiffness matrix, mass matrix,and load case vectors to afile.These options are described later in this section.A single analysis can include multiple substructure generate steps,and Abaqus/CAE createscorresponding output databasefiles for each step.Multiple preloading steps can precede everySPECIFYING THE RETAINED NODAL DEGREES OF FREEDOM AND LOADCASES FOR A SUBSTRUCTURE substructure generation step in your analysis.If you want to specify retained eigenmodes forsubstructure generation,you must also include a frequency extraction step in the analysis.Substructure identifierYou must specify a unique identifier for each substructure you create.Substructure identifiers must begin with the letter Z followed by a number that cannot exceed999.Recovery optionsYou can recover thefield output data for a substructure during the usage-level analysis,but you must specify the recovery region during substructure generation.Substructure recovery can be performed only on the sets included in the recovery region.You can specify that recovery be performed on the whole model or for an individual node set or element set.While performing the substructure recovery in the usage model,Abaqus/CAE must have access to the substructure’s.mdl,.prt, .stt,and.supfiles.For more information about thesefile types,see“Defining substructures,”Section10.1.2of the Abaqus Analysis User’s Manual.Generation optionsYou can control several aspects of the substructure generation process,including calculation of gravity load vectors,evaluation of frequency-dependent material properties,and generation of a reduced mass matrix,reduced structural damping matrix,and viscous damping matrix.Retained eigenmodesYou can specify retained eigenmodes for generation of a coupled acoustic-structural substructure.When you choose to specify retained eigenmodes,Abaqus/CAE enables you to specify eigenmodes by mode range or by frequency range.DampingYou can specify several global damping controls and substructure damping controls.For global damping you can choose to apply damping settings to acoustic or mechanical options;for substructure damping you can specify separate controls for viscous and structural damping. 39.3Specifying the retained nodal degrees of freedom and load casesfor a substructureAfter you defined the substructure generation step or steps for your analysis,you must define a Retained nodal dofs boundary condition for a substructure.The retained degrees of freedom for a substructure node are the degrees of freedom that are external and are available for use in the analysis;all other degrees of freedom for the specified node are assumed to be internal to the substructure and do not factor into the analysis.When you import a substructure from this analysis into a model for substructure usage, Abaqus/CAE displays these nodes as light blue crosses,which enables you to pick them easily from a part instance or assembly.ACTIVA TING LOAD CASES DURING SUBSTRUCTURE USAGEIf you want to apply a load to the substructure at a location other than its retained degrees of freedom, you can define a load case in the substructure generation step.39.4Importing a substructure into Abaqus/CAEYou can include substructure definitions in a model database and begin to use them for modeling by importing the substructures as new part definitions.Substructure data are available in.simfiles, and the substructure identifier is included in thefile name;for example,in an analysis in which the substructure is named FAN and the substructure identifier is Z400,the substructure databasefile is named FAN_Z400.sim.The.simfile from which you import a substructure must reside in the same directory as the supporting Abaqusfiles to which the.sim database refers;these supportingfiles may include data in the formats.prt,.mdl,.stt,or.sup.Substructure import also requires an output database(.odb)file for mesh display.39.5Using substructure part instances in an assemblyOnce you import substructure parts into your model database,you can add them to your assembly by instancing them in the same manner you would for any part.Substructure part instances are displayed in a translucent color in the viewport.You can move and apply constraints to substructure part instances;however,substructure part instances have the following modeling limitations:•You cannot assign sections to a substructure part instance.•You cannot apply attributes to a substructure part instance.•Substructure part instances are not eligible for definition of contact pairs.•Gravity loads are the only load definition that can be applied to substructure part instances. 39.6Activating load cases during substructure usageThe Substructure load definition enables you to activate the substructure load cases that are specified during the substructure generation step.As you activate a load case,you can scale its load definitions or apply an amplitude to them.VISUALIZING SUBSTRUCTURE OUTPUT39.7Recovering field output for substructuresYou can specify that Abaqus/CAE writefield output data for one or more substructure sets in your analysis.From thefield output editor,select Substructure from the Domainfield,then click to open the Select Substructure Sets dialog box.This dialog box lists only the substructure sets that were defined while generating the substructure.You cannot recover data for sets that you define on substructure part instances in Abaqus/CAE.39.8Visualizing substructure outputAbaqus/CAE creates separate output database(.odb)files for each substructure part instance used in the analysis,so you must perform some additional steps if you want to display substructure results in context with the rest of the assembly.The Visualization module provides the following tools that enable you to incorporate substructure results into the rest of the model:•You can use an overlay plot to display plots of substructure data in the same viewport as a plot of the rest of the assembly.•You can use the Combine ODBs plug-in to combine the data in one or more substructure output databasefiles with the data from the rest of the assembly.。