Bulk Data Entry Defines the CMS (Component Mode Synthesis) method, frequency upper limit, number of modes, and starting SPOINT ID to be used in a CMS solution.

The eigenvalue solver is also specified. In addition, preload as well as loads for reduction and residual vector generation can be defined. Also, an ASCII file containing CELAS4 and CDAMP3 element data and/or their corresponding design variable definitions can be generated for DMIG to allow the use of the component modes in optimization runs.


(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
Optional continuation lines for Fluid Analysis (mandatory if a minimum of 1 Fluid grid is present in the model)
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
Optional continuation lines for preload definition
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
Optional continuation lines for LOADSET definition
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
Optional continuation lines for DMIGDV definition
(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)


(1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
CMSMETH 5 CBN 1000 200 100000
+ 600 100 200000


Field Contents SI Unit Example
CMSID CMSMETH identification number.

(Integer > 0)

METHOD Component Mode Synthesis method to be employed. 2

No default (Character)

UB_FREQ Upper bound frequency for the eigenvalue analysis for the structural part.
0.0 or blank
No upper bound is used. 3 4

Default = blank (Real > 0.0, or blank)

NMODES Number of modes to be extracted from structural eigenvalue analysis.
-1 or blank
Number of modes is limitless. 3 4

Default = blank (Integer > -1, or blank)

SPID The starting SPOINT ID to be used in DMIG matrix output for the structural eigenmodes.

No default 6

SOLVER The eigenvalue solver.
LAN (Default)


AMPFFACT AMSES Amplification Factor. The substructure modes are solved up to the frequency of AMPFFACT*V2. Higher values of AMPFFACT will lead to more accurate results and longer running times. 9

Default = 5.0 (Real or blank)

SHFSCL For vibration analysis, it is the estimate of the frequency of the first flexible mode. 12

Default = blank (Real or blank)

UB_FREQ_F Upper bound frequency for the eigenvalue analysis for the fluid part. If 0.0 or blank, no upper bound is used. 3 4

Default = blank (Real > 0.0, or blank)

NMODES_F Number of modes to be extracted from fluid eigenvalue analysis. If set to -1 or blank, number of modes is limitless. 3 4

Default = blank (Integer > -1, or blank)

SPID_F The starting SPOINT ID to be used in DMIG matrix output for the fluid eigenmodes.

No default 6

GPRC Grid participation recovery control.

Allows fluid-structure interface grid shape data (that is the modes associated with the fluid-structure interface) to be calculated and stored with the external superelement.

Only applicable when GM (general modal formulation) is input in the METHOD field and when all boundary degrees-of-freedom are free (BNDFREE).

If any boundary degrees-of-freedom are fixed and GPRC is set to YES, the program will be terminated with an error.

Default = NO (YES or NO)

PRELOAD Flag indicating that a preload will be used in the CMS analysis. 21
SPCID SPC SET ID for the preload.
PLSID LOAD SET ID for defining the preload.
LOADSET Flag indicating that static loads will be reduced in CMS superelement generation run. 11 19
USETYPE Static loads reduction type. 11 19
Loads defined on the LSIDi fields are used for generating residual vectors to improve the modal space.
Loads defined on the LSIDi fields used for generating reduced loads.
BOTH (Default)
Both RESVEC and REDLOAD options are selected.
LSIDi The static load IDs for generating residual vectors and/or reduced loads.
S Selects the structural part of the model. 25

Default = S

DMIGDV Flag indicating that an ASCII file containing CELAS4 and CDAMP3 element data and/or their corresponding design variable definitions is generated for DMIG. 13
OUTOPT Defines how design variable definitions are written for DMIG. 13 17
Only CELAS4 and CDAMP3 element data and PDAMP properties (if any) are written. Design variable definitions are not written.
All data from Option -1 and design variable definitions are written. 14
All data from Option -2 and constraint (f1<f2) creation data are written. 15
Option -2 is the default.
NMODE Defines the number of design variables for ΔK/ΔGE and ΔB in CELAS4 and CDAMP3. 18
> 0
The "NMODE" number of design variables will be written to control the first "NMODE" eigenvalue changes (ΔK), damping coefficient changes (ΔGE) and scalar damping value changes (ΔB).
As many design variables as the total number of modes are written.
DVKUPFAC Used to determine the upper bound of ΔK (which is (maximum eigenvalue)*DVKUPFAC). If DVKUPFAC is not specified (DVKUPFAC field is blank). 16

Default: DVKUPFAC=0.1

DVGEUP Upper bound of ΔGE. This applies to all the design variables for ΔGE. If DVGEUP is not specified (DVGEUP field is blank), by default it is set to 2*DVBUP. 16


DVBUP Upper bound of ΔB. This applies to all the design variables for ΔB. If DVBUP is not specified (DVBUP field is blank). 16

Default: DVBUP=0.4


  1. This definition will be ignored unless referenced in the I/O Options section by a CMSMETH run control.
  2. Several methods are available for Component Mode Synthesis, these are: CB, CC, CBN, GM and GUYAN (see descriptions below).

    Depending on the type of input required by the Multibody Dynamics Solvers, different methods can be used to generate the flexible body representations. For example, the CB and CC methods are used for generating flexible bodies for use with some Multibody dynamics solvers, like MotionSolve. The CBN method can be used to generate CMS superelement information for some third-party solvers (see Create Output for Third Party Software for more information). Additionally, some of these methods (CBN, GM, GUYAN) can be used to generate external superelements (stored in DMIG format) for use in subsequent finite element analyses.

    GUYAN is the same as CBN without including structural eigenmodes; when GUYAN is used, UB_FREQ and NMODES are ignored.

  3. UB_FREQ, NMODES, UB_FREQ_F and NMODES_F cannot all be blank. Additionally, when structural elements are present in the model, UB_FREQ and NMODES cannot both be blank, and when fluid elements are present in the model, UB_FREQ_F and NMODES_F cannot both be blank.
  4. When UB_FREQ = 0.0 and NMODES = 0, this is a special case where no structural eigenmodes will be included in CMS mode generation. If both UB_FREQ and NMODES are specified, lowest NMODES below UB_FREQ will be accepted as structural SPOINTs. Similarly things are applied to fluid part.
  5. If PARAM, EXTOUT, DMIGPCH (or DMGBIN) is defined when using the CBN method, a DMIG matrix corresponding to the reduced stiffness and mass matrices will be output. The stiffness and mass corresponding to the eigenmodes will be assigned to the generated SPOINTs.
  6. The SPOINT IDs of the structure and fluid should have distinct IDs. Any fluid SPOINT ID cannot be in between structural SPOINT IDs.
  7. When PARAM,EXTOUT is used to output DMIG matrices, then it is possible to disable the output of a flexh3d file by specifying "OUTPUT,H3D,NONE" in the input file.
  8. The nodal flexh3d file output from the CBN method can be used as the DMIG input (using ASSIGN,H3DDMIG). In this way, the model set output in flexh3d file will be recovered as the interior points of the DMIG matrix in the residual structure run. The displacements of these interior points will be included in the output.
  9. AMPFFACT is used to increase the accuracy of the eigenvalue and eigenvectors at the expense of slightly longer run times. It is recommended to use higher values of AMPFFACT for solid structures like engine blocks and suspension components. If AMPFFACT is not specified by you and the model contains a large number of solid elements, the value of AMPFFACT is automatically reset to 10.
  10. The mass properties of the super element (Mass, Center of Gravity, and Moments of Inertia) are written to the H3D file. In the residual run, these mass properties are included in the mass properties of the structure printed in the .out file.
  11. Static load reduction is supported for CMSMETH superelement generation runs (METHOD=CBN/GUYAN) and Flexbody generation runs (METHOD=CB/CC). Static load reduction is not supported for GM superelement generation runs.
  12. A specification of SHFSCL may improve the performance of a vibration analysis.
  13. If the DMIGDV optional continuation card is defined, a text file (ASCII) is created after the run. This file can be included in the original input deck to study how changes in the eigenvalues/damping of superelements affect the performance of the residual structure.
  14. In addition to the data included in option 1, the ASCII file now also contains design variable definitions. These design variables can control available eigenvalues, structural damping, and viscous damping of the superelement. You can set up an optimization problem by including this file in the original input deck.
  15. In addition to the data included in option 2, the ASCII file now includes data required for the creation of constraints. These constraints ensure that the eigenvalue of the nth mode is less than the eigenvalue of the (n+1)th mode during optimization.
  16. The lower bound of ΔK, ΔB and ΔGE is set such that K, B and GE are always greater than or equal to zero.
  17. The DMIGDV continuation line works only for METHOD = GM (General Modal formulation) in field 3 of CMSMETH. 2
  18. Where, ΔK, ΔGE and ΔB represent increments/decrements to the eigenvalues (K), damping coefficients (GE) and scalar damping values (B), respectively. It is required to include the .h3d file containing the values of K, GE and B using ASSIGN, H3DDMIG.
  19. The LOADSET flag is required only for the first continuation line. Multiple continuation lines with LSID's do not require the LOADSET flag.
  20. For further information on creating flex bodies for third party software, refer to Create Output for Third Party Software in the User Guide.
  21. Preloading for Component Mode Synthesis subcases can now be defined using the STATSUB(PRELOAD)=SID command. This is more versatile than the PRELOAD continuation line, as any static subcase can be applied as a preload.
  22. SDAMPING cannot be included in the generation of CMS superelements. SDAMPING can be included in the generation of CDS superelements (CDSMETH entry). If you used SDAMPING in the generation of the combined CDS and CMS (METHOD=GM) superelements, the SDAMPING will be included only in the CDS superelement. Use DMIGMOD to apply SDAMPING in the residual run to the CMS (METHOD=GM) superelements. If SDAMPING is not required for CMS superelements in the residual run, then the corresponding DMIGMOD data can be excluded from the model.
  23. CMS runs are not supported, if Frequency-dependent materials are present in the model.
  24. PUNCH output files generated from CMS runs contain ASET, BSET, and CSET information and their corresponding grid and coordinate systems along with the SPOINTs corresponding to the structural eigenmodes.
  25. Currently, the fluid part of the model cannot be selected for the DMIGDV continuation line on the S field.
  26. For flexbody H3D file generation via the CC and CB methods, the H3D is always output in Kg,N,mm,s unit system. You can define the units of the FE model in OptiStruct via the UNITS or DTI,UNITS entry. Refer to Unit Systems for more information.
  27. For CMS reduction, viscous damping via CVISC, CDAMPi, CBUSH (via B on PBUSH) can be reduced in the generation run. However, viscous damping via SDAMPING is not reduced. Global Rayleigh damping via PARAM,ALPHA1 and PARAM,ALPHA2 is reduced as of OptiStruct 2022, when PARAM,CMSGDMP,YES is specified.

    Structural damping via GE on MATi, PBUSH with GE, and PELAS with GE are reduced in the generation run. Global structural damping via PARAM,G is reduced as of OptiStruct 2022 when PARAM,CMSGDMP,YES is specified.

    For more information, refer to Direct Matrix Input (Superelements) in the User Guide.

  28. This card is represented as a load collector in HyperMesh.