The generation pass is where you condense a group of "regular" finite elements into a single superelement. The condensation is done by identifying a set of master degrees of freedom, used mainly to define the interface between the superelement and other elements and to capture dynamic characteristics for dynamic analyses. Figure 2.2: Example of a Substructuring Application shows a plate-like structure that is to be analyzed with contact (interface) elements. Since the contact elements require an iterative solution, substructuring the plate portion can result in a significant savings in computer time. The master DOF required in this case are the degrees of freedom that connect the plate to the contact elements.
Generating a superelement involves two primary tasks:
In this step, you specify the jobname and analysis title and then use /PREP7 to define the element types, element real constants, material properties, and the model geometry. These tasks are common to most analyses and are described in the Basic Analysis Guide. For the generation pass, you should keep in mind the following additional points:
Jobname-This takes on special significance in a substructure analysis. By using jobnames effectively, you can eliminate much of the file handling inherent in a three-pass analysis.
Use one of these methods to specify the jobname:
For example,
/FILNAME,GEN
gives the jobname GEN to all files produced by the generation pass. The default jobname is file or whatever name was specified while entering the program.
Element Types - Most element types can be used to generate a substructure. In general, the only restriction is that elements within the superelement are assumed to be linear and cannot use Lagrange multipliers. If you include bilinear elements, they will be treated as linear elements (in their initial state).
Caution: Coupled-field elements used in a direct method coupled-field analysis with load vector coupling are not valid in a substructure analysis. Other elements in the same shape family should be used instead. See the Coupled-Field Analysis Guide for details. In addition, elements with Lagrange multipliers cannot be used in substructuring. These type of elements include MPC184, CONTA171, CONTA172, CONTA173, CONTA174, CONTA175, CONTA176, CONTA177, and CONTA178 with appropriate KEYOPT(2) setting, and elements PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, SOLID272, SOLID273, and SOLID285 when using KEYOPT(6) > 0.
Material Properties - Define all necessary material properties. For example, if the mass matrix is to be generated, density (DENS) (or mass in some form) must be defined; if the specific heat matrix is to be generated, the specific heat (C) must be defined; and so on. Again, because a superelement is linear, any nonlinear material properties will be ignored.
Model Generation - In the generation pass, you are mainly concerned with creating the superelement portion of the model. The nonsuperelement portion, if any, is defined later in the use pass. However, you should plan the modeling approach for both portions before you start building the model. In particular, decide on how you want to connect the superelement to the other elements. To ensure the connection, use the same node numbers at the interface. (Other methods requiring less effort on your part are discussed in the use pass section later in this chapter.)
Edge Outline - Adjust the edge outline used to plot the superelement in the use pass [/EDGE]. A smaller angle will produce more edges.
One approach might be to develop the entire model, save it on a named database file, and select only the portion to be substructured for the generation pass. In the use pass then, you can RESUME () from the named database file, unselect the portion that was substructured and replace it with the superelement matrix. The top-down approach is described in Top-Down Substructuring.
The "solution" from a substructure generation pass consists of the superelement matrix (or matrices). As with any other analysis, you define the analysis type and options, apply loads, specify load step options, and initiate the solution. Details of how to do these tasks are explained below.
Enter SOLUTION using either of these methods
Define the analysis type and analysis options The applicable options are explained below.
Analysis Type - Choose a substructure generation using one of these methods:
New analysis or restart - If you are starting a
new analysis, choosing the analysis type (as described above) is all you need to do.
However, if the run is a restart, you must also indicate this by setting
STATUS = REST on the ANTYPE
command (). A
restart is applicable if you need to generate additional superelement load vectors.
(The files Jobname.ESAV and Jobname.DB
from the initial run must be available for the restart.
The Jobname.EMAT file is also required if it was created in the initial
run.)
Note: Restarting a substructure analysis is valid only if the backsubstitution method is chosen. You cannot restart a run if the full resolve option is selected using the SEOPT command.
Name of the superelement matrix file - Specify
the name (Sename) to be assigned to the superelement
matrix file. The program will automatically assign the extension SUB, so the
complete file name will be
Sename.SUB. The default is to
use the jobname [/FILNAME]. To specify the name of the
superelement matrix file:
Equation Solver - The SPARSE solver is the only solver available for the generation pass of the substructure analysis.
Matrices to be generated - You can request generation of just the reduced stiffness matrix (or conductivity matrix); stiffness and mass matrices (or specific heat); or stiffness, mass, and damping matrices. The mass matrix is required if the use pass is a structural dynamic analysis or if you need to apply inertia loads in the use pass. For the thermal case, the specific heat matrix is required only if the use pass is a transient thermal analysis. Similar considerations apply to other disciplines and to the damping matrix. To make your request, use the SEOPT command as described above.
Note: You should verify that damping is present in the substructure model when using
SEMATR = 3 on the SEOPT
command. If not, a null reduced damping matrix is generated and stored in the
associated .SUB file, which can increase the size of the
file.
For first-order non-structural analysis types (thermal, electric, magnetic,
diffusion), whereas the matrix associated with the first-order DOFs (for
instance, specific heat for thermal analysis) is the equivalent of a damping
matrix in structural analysis, the reduction of all matrices is specified with
SEMATR = 2 on the SEOPT
command. For coupled-field analyses, only the reduction of the stiffness matrix
(or the equivalent matrix) is possible.
Matrices to be printed - This option allows you to print out the superelement matrices. You can request listing of both matrices and load vectors, or just the load vectors. The default is not to print any matrices. To print out the matrices, use the SEOPT command:
Expansion Pass Method - Allows you to select the expansion pass method you plan to use during subsequent expansion passes with this superelement. The backsubstitution method (default) saves the factorized matrix files needed to perform a backsubstitution of the master DOF solution during the expansion pass. The full resolve method does not save any factorized matrix files. The factorized matrix files are named Sename.LNxx for the sparse solver.
Note: Factorized matrix files can become very large as the problem size increases, but are not needed if the full resolve method is chosen during the expansion pass.
During the expansion pass, the full resolve method reforms the elements used to create the superelement, reassembles the global stiffness matrix, and applies the master DOF solution as displacement boundary conditions internally. These displacement boundary conditions are deleted upon finishing the expansion pass solution.
Note: You cannot restart a substructure analysis with the full resolve expansion pass method chosen.
Mass matrix formulation - Applicable only if you want the mass matrix to be generated. You can choose between the default formulation (which depends on the element type) and a lumped mass approximation. We recommend the default formulation for most applications. However, for dynamic analyses involving "skinny" structures, such as slender beams or very thin shells, the lumped mass approximation has been shown to give better results. To specify a lumped mass approximation, use one of these methods:
Modes to be used - For superelements being used in a subsequent dynamic analysis [ANTYPE,MODAL, HARMONIC, or TRANSIENT], you may include mode shapes as extra degrees of freedom to obtain better accuracy [CMSOPT]. See the chapter on Component Mode Synthesis for more information.
Define master degrees of freedom using one of these methods
In a substructure, master DOFs serve three purposes:
They serve as the interface between the superelement and other elements.
Be sure to define master DOFs at all nodes that connect to nonsuperelements,
as shown in Figure 2.2: Example of a Substructuring Application. All degrees of freedom at these nodes should be defined as
master DOFs (Lab = ALL on the
M command). Master DOFs must be defined even if you
plan to have no elements in the model other than a superelement.
If the superelement is to be used in a dynamic analysis, master DOFs characterize the dynamic behavior of the structure if the Component Mode Synthesis method [CMSOPT] is not used. See Modal Analysis in the Structural Analysis Guide for guidelines.
If constraints [D] or force loads [F] are to be applied in the use pass, master DOFs must be defined at those locations with the M command.
If this superelement is to be transformed [SETRAN] later in the use pass or used in a large deflection analysis [NLGEOM,ON], then all nodes that have master DOFs must have all six DOFs (UX, UY, UZ, ROTX, ROTY, ROTZ) defined and active.
For large deflections, master DOFs are typically defined at the joints of the flexible body and are at the nodes connected to a joint element (MPC184), another rigid or flexible body node, or ground. At least two master DOFs must be defined for each substructure, as the average rotation of the superelement is computed from the average rotation of its master DOF. If only one node is a joint node, then another must be chosen at the free end. See the Multibody Analysis Guide for more details.
You can apply all types of loads in a substructure generation pass. Some types of loading involve certain considerations, as follows:
The program generates a load vector that includes the effect of all applied loads. One superelement load vector per load step is written to the superelement matrix file. This load vector represents the combination of the loads defined during the load step.
The maximum number of load vectors that can be generated and stored in
the Sename.sub file defaults to 1000. To increase
this limit, the /CONFIG command with
Lab = NUMSUBLV can be used.
Nonzero degree of freedom constraints can be used in the generation pass and will become part of the load vector.
In the expansion pass, if the load step being expanded contains nonzero degree of freedom constraints, the database must have matching degree of freedom values. If it does not, the degree of freedom constraints must be specified [D] again in the expansion pass.
Application of constraints [D] or force loads [F] can be postponed until the use pass, but a master degree of freedom must be defined at those locations with the M command or corresponding GUI path.
If a mass matrix is generated, apply the degree of freedom constraints in the use pass at the master degree of freedom (defined in the generation pass) to ensure that all mass is accounted for in the substructure. For analyses with acceleration loadings, the load should be applied in the generation pass and used in the use pass for greater accuracy, rather than apply the acceleration load on the reduced mass matrix.
Similarly, application of linear and angular accelerations can be postponed until the use pass, but only if a mass matrix is generated. A postponement is desirable if you plan to rotate the superelement in the use pass, because load vector directions are "frozen" and rotated with the superelement.
The Maxwell force flag (MXWF label on the SF family of commands) is normally used in a magnetic analysis to flag element surfaces on which the magnetic force distribution is to be calculated. The flag has no effect (and therefore should not be used) for a superelement in a magnetic analysis.
If you intend to create an imaginary force vector, generate it as a
real load vector, then use it as an imaginary load vector in the use pass
(SFE,,,,KVAL = 2) and
expansion pass
(SEEXP,,,ImagKy =
ON).
When a load vector exists for a thermal superelement, it must be applied and have a scale factor of 1 (SFE,,,,,SELV,,1).
For large-rotation analyses, do not apply constraints to the model in this pass, as you will apply constraints for large rotation analyses in the use pass.
Table 2.1: Substructure Analysis Loads
| Load Name | Load Category | Commands[1] | |
|---|---|---|---|
| Solid Model Loads | Finite Element Loads | ||
| Displacement Temperature Mag. Potential ... | Constraints | DK, DKLIST, DKDELE, DL, DLLIST, DLDELE, DA, DALIST, DADELE, DTRAN | D, DSYM, DLIST, DDELE, DSCALE, DCUM |
| Force Heat Flow Rate Mag. Flux ... | Forces | FK, FKLIST, FKDELE, FTRAN | F, FLIST, FDELE, FSCALE, FCUM |
| Pressure Convection Maxwell Surface ... | Surface Loads | SFL, SFLLIST, SFLDELE, SFA, SFALIST, SFADELE, SFGRAD, SFTRAN | SF, SFLIST, SFDELE, SFE, SFELIST, SFEDELE, SFBEAM, SFGRAD, SFFUN, SFSCALE, SFCUM |
| Temperature Heat Generation Rate Current Density ... | Body Loads | BFK, BFKLIST, BFKDELE, BFL, BFLLIST, BFLDELE, BFA, BFALIST, BFADELE, BFV, BFVLIST, BFVDELE, BFTRAN | BF, BFLIST, BFDELE, BFE, BFELIST, BFEDELE, BFSCALE, BFCUM |
| Gravity, Linear and Angular Acceleration | Inertia Loads | ACEL, DOMEGA | |
The menu path used to access each command in the GUI will vary depending on the engineering discipline of the analysis (structural, magnetic, etc.). For a list of menu paths, see the description of individual commands in the Command Reference.
Specify load step options The only options valid for the substructure generation pass are dynamics options (damping).
Damping (Dynamics Options) - Applicable only if the damping matrix is to be generated.
To specify damping in the form of alpha (mass) damping:
To specify damping in the form of beta (stiffness) damping:
To specify damping in the form of material-dependent alpha damping:
To specify damping in the form of material-dependent beta damping:
Save a backup copy of the database on a named file Doing this is required because you need to work with the same database in the expansion pass. To save a backup copy, use one of these methods:
Start solution calculations using one of these methods:
Sename.SUB,
where Sename is the name assigned as an
analysis option [SEOPT] or the jobname
[/FILNAME]. The matrix file includes a load
vector calculated based on the applied loads. (The load vector will
be zero if no loads are defined.) Repeat for additional load steps (that is, to generate additional superelement load vectors) The superelement load vectors are numbered sequentially (starting from 1) and appended to the superelement matrix file. See Loading in the Basic Analysis Guide for other methods for multiple load steps.
Leave SOLUTION using one of these methods