The following sections describe the CMS generation pass:
The process for generating a CMS superelement consists of two primary tasks:
Building the model
This step is identical to building the model for a substructuring analysis. Define density (DENS)--or mass in some form--because CMS must generate both stiffness and mass matrices.
Creating the superelement matrices
The "solution" from a CMS generation pass consists of the superelement matrices (reduced stiffness and mass matrices or reduced stiffness, mass, and damping matrices). This flowchart illustrates the process necessary for creating the superelement matrix file:
Specifying the CMS method When specifying the CMS method, also specify the number of modes and, optionally, the frequency range used to generate the superelement. The program supports the fixed-interface (CMSOPT,FIX), free-interface (CMSOPT,FREE), and residual-flexible free-interface (CMSOPT,RFFB) CMS methods. If using the free-interface method, also specify the rigid body modes (CMSOPT,,,,FBDDEF). If using the residual-flexible free-interface method, specify pseudo-constraints (D,,,SUPPORT).
Specifying the mode-extraction method The default method is Block Lanczos
(EIGMETH = LANB on
CMSOPT). The Subspace and Supernode methods are
also supported. See Comparing Mode-Extraction Methods in the Mechanical APDL Structural Analysis Guide for a comparison of the methods. When
using the Supernode mode-extraction method
(EIGMETH = SNODE), the frequency range
specified by the
FREQB/FREQE
arguments defaults to 0-100 Hz, similar to the MODOPT
command behavior for this eigensolver. Therefore, it is important to
properly define the input quantities when using the Supernode method in
order to achieve good performance and accuracy.
Naming the superelement matrix file The program assigns the .sub extension to the
superelement matrix file name that you specify
(SEOPT,Sename);
therefore, the complete file name is Sename.SUB. The default file name is the
Jobname (/FILNAME).
Specifying the lumped mass matrix formulation Specify the lumped mass matrix formulation (LUMPM) if necessary. For most applications, ANSYS, Inc. recommends the default formulation (depending upon the element type); however, for dynamic analyses involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation typically yields better results.
Defining master DOFs In a substructure, master degrees of freedom (DOFs) serve as the
interface between the superelements or other elements. Define master
DOFs (M) at all nodes that connect to
non-superelements (Lab1 = ALL), as shown in
Example of a Substructuring
Application. You must define master
DOFs even if you intend to have no elements in the model other than
a superelement.
If constraints (D) or force loads (F) are to be applied in the use pass, master DOFs must be defined at these locations with the M command. Nevertheless, if the fixed-interface CMS method (CMSOPT,FIX) is used, the load should be applied in the generation pass and used in the use pass as a load vector to avoid over-constrained fixed-interface normal modes.
If this superelement is to be transformed (SETRAN) later in the use pass or used in a large deflection analysis (NLGEOM,ON), 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.
Specifying pseudo-constraints Required for the residual-flexible free-interface method (CMSOPT,RFFB). For each superelement where rigid-body modes exist, specify pseudo-constraints. Apply only the minimum number of displacement constraints (D,,,SUPPORT) necessary to prevent rigid body motion: three constraints (or fewer, depending on the element type) for 2-D models and six (or fewer) for 3-D models.
Saving a copy of the database Saving a copy of the database (SAVE) is necessary because you must work with the same data in the expansion pass.
Obtaining the CMS generation pass solution Output from the solution (SOLVE) consists of the
superelement matrix file (Sename.SUB), where
Sename is the file name you assigned (via
the SEOPT command).
As in a substructure generation pass, multiple superelement load vectors can be generated in a CMS generation pass by issuing multiple SOLVE commands. This can also be done in a restart of the CMS generation pass (ANTYPE,SUBSTR,RESTART).
Nested superelements cannot be generated with a CMS generation pass using the residual-flexible free-interface CMS method.
The RESVEC,ON command can be issued in the first load step to calculate one residual vector which is included in the normal modes basis used in the transformation matrix of the three available CMS methods.
When the Coriolis effect in the stationary reference frame is activated (CORIOLIS,ON,,,ON), the stiffness, mass, and damping matrices are treated as non-symmetric by the sparse solver in the generation pass. This doubles the amount of memory used when compared to symmetric systems. For a model with a large number of degrees of freedom, the memory options for the sparse solver (BCSOPTION) should be set using the guidelines outlined in Direct (Sparse) Solver Memory Usage in the Performance Guide.
After obtaining the CMS superelement matrices, proceed to the use pass and then the expansion pass, as you would in a substructuring analysis.
For a detailed example of how to use CMS, see Modal Analysis of a 2-D Tuning Fork.
The following table describes the different types of component modes that make up the transformation matrix for the three CMS methods, as described in Component Mode Synthesis (CMS) in the Mechanical APDL Theory Reference. It also defines the CST, IRF, NOR, and RSD abbreviations.
Table 3.1: Component Modes Definition
| FIX | FREE | RFFB | |
|---|---|---|---|
| Constraint mode data (CST) |
where | same as FIX | – |
| Inertia relief mode data (IRF) | – |
where | – |
| Fixed-interface normal mode data (NOR) |
|
where |
where |
| Residual attachment mode data (RSD) | – | – |
|
The modes described in Table 3.1: Component Modes Definition are written to the
.CMS and .TCMS files during the
generation pass. The format of these files is described in CMS File Format and TCMS File Format in the
Programmer's Reference. By default the static constraint modes are not written to the
.CMS file for the fixed-interface and free-interface
methods. Issue CMSOPT with IOKEY = CMS
to write them.
If the CMSOPT command is issued with
IOKEY = TCMS, the transformation matrix is printed
out and written to the .TCMS file. This will only occur if the
OUTPR is issued with ITEM = NSOL
and FREQ not equal to NONE.
The following table summarizes the contents of the .CMS and .TCMS files. It also specifies the degrees of freedom ordering of the component modes. See Degree of Freedom Ordering in the ANSYS Parametric Design Language Guide for more information on degree of freedom ordering.
Table 3.2: Contents of .CMS and .TCMS Files and DOF Ordering According to IOKEY Setting
| FIX | FREE | RFFB | |||||
|---|---|---|---|---|---|---|---|
| CST | NOR | CST | IRF | NOR | RSD | NOR | |
| .CMS File | DOFs ordering: solver | DOFs ordering: internal | |||||
IOKEY ≠ CMS | No | Yes | No | Yes | Yes | Yes | Yes |
IOKEY = CMS | Yes | Yes | Yes | Yes | Yes | Yes | Yes |
| .TCMS File | DOFs ordering: user | – | |||||
IOKEY = CMS | Yes | Yes | Yes | Yes | Yes | – | – |
By default, in the expansion pass, and for each solution, the expansion of nodal DOF displacements is followed by the calculation of element results such as nodal loads, reaction loads, and energies. No element results calculation is performed in the generation pass.
The CMS fixed-interface method supports the element results calculation during the
generation pass. If ELCALC is set to YES on the
CMSOPT command (CMSOPT,FIX,,,,,,,,YES),
the element results of each static constraint mode and each fixed-interface mode are
written to the .CMS file and then directly combined during the
expansion pass. For more information, see Component Mode Synthesis (CMS) in the
Mechanical APDL Theory Reference.
This procedure reduces the computation time of the expansion pass if:
| The number of solutions to expand is high (typically hundreds), and |
| The number of master DOFs is low compared to the total number of DOFs of the substructure model (typically less than 100 master DOFs for a finite element model with 150000 DOFs). |
This procedure has the following limitations:
It is only supported by the CMS fixed-interface method
(CMSMETH = FIX on
CMSOPT)
The element nodal loads are available only if there is at least one load applied during the generation pass
Reaction forces are available only if degrees of freedom constraints are specified in the generation pass
Note: In general, this is not advisable as the mass matrix is not entirely accounted for in the superelement matrix.
Following a transient analysis or a harmonic analysis use pass, quantities
using nodal velocities and nodal accelerations (damping force, inertial
force, kinetic energy, etc.) can be computed and postprocessed only if the
OUTRES command was issued in the first load step of
the use pass with DSUBres = ALL
The damping element forces and reaction forces are available if a damping matrix was assembled in the generation pass. Damping results do not take into account the damping added during the use pass
Equivalent strains are evaluated using EFFNU =
0.0. Use AVPRIN to set the appropriate Poisson's ratio
value
Thermal loads are not supported
NMISC results are not available
Strains and stresses of PIPE elements are not available in the expansion pass
Acoustic elements are not supported in the generation pass
Linear perturbation analysis substructure generation pass is not supported
The usage of SETRAN or SESYMM in the
use pass is not supported if the original superelement matrix was created
with ELCALC = YES on
CMSOPT
Nested superelements cannot be generated from an original superelement
matrix created with ELCALC = YES on
CMSOPT
If ELCALC = YES on CMSOPT, the
factorized matrix files SEname.LNxx are not required for the
expansion pass. Consequently, if restarting the generation pass is not required,
ExpMth can be set to NONE on SEOPT
to save disk space.