3.1. The CMS Generation Pass

The following sections describe the CMS generation pass:

3.1.1. Creating the Superelement

The process for generating a CMS superelement consists of two primary tasks:

  1. 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.

  2. 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:

    Figure 3.1:  Process Flow for Creating a CMS Superelement Matrix

    Process Flow for Creating a CMS Superelement Matrix

    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.

3.1.2. Component Modes Storage

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

 FIXFREERFFB
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

 FIXFREERFFB
 CSTNORCSTIRFNORRSDNOR
.CMS FileDOFs ordering: solverDOFs ordering: internal
IOKEY ≠ CMSNoYesNoYesYesYesYes
IOKEY = CMSYesYesYesYesYesYesYes
.TCMS FileDOFs ordering: user–
IOKEY = CMSYesYesYesYesYes––

3.1.3. Calculating the Element Results

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.


Release 18.2 - © ANSYS, Inc. All rights reserved.