Archive Documentation
The reduced modal analysis is an archived feature requiring use of the following command:
MODOPT, Method,
NMODE, FREQB,
FREQE, PRMODE,
Nrmkey, --,
BlockSize, --,
--, Scalekey .
For a reduced modal analysis, use the MODOPT command as described in the Command Reference with the following exceptions:
Set Method = REDUC.
For the reduced method, NMODE defaults to the
number of master DOFs. It is recommended that you set
NMODE to less than half of the number of
master DOFs.
PRMODE is the number of reduced modes to
print.
To perform a reduced modal analysis, follow the general procedures outlined in Modal Analysis in the Structural Analysis Guide.
During the step “Define Analysis Type and Options”, follow these instructions for a reduced modal analysis:
When specifying the mode extraction method, issue the command MODOPT,REDUC to specify the reduced (Householder) mode extraction method.
Define master degrees of freedom (M and MGEN commands).
Master degrees of freedom (MDOFs) are significant degrees of freedom that characterize the dynamic behavior of the structure. Generally, you should select at least twice as many MDOFs as the number of modes of interest. ANSYS, Inc. recommends that you define as many MDOFs as you can, based on your knowledge of the dynamic characteristics of the structure. You can list the defined MDOFs (MLIST) and delete extraneous MDOFs (MDELE).
The following example input demonstrates a typical modal analysis procedure:
/PREP7 /TITLE, VIBRATION OF A FLUID COUPLING C*** USING HARMONIC FLUID ELEMENTS (FLUID81) C*** (FLUID81 IS AN ARCHIVED ELEMENT) ANTYPE,MODAL ! MODE-FREQUENCY ANALYSIS MODOPT,REDUC ET,1,FLUID81 ET,2,COMBIN14,,,2 ! 2-D LONGITUDINAL SPRING R,2,10 ! HARMONIC SPRING CONSTANT MP,EX,1,3E5 MP,DENS,1,934E-7 N,1,7 N,2,8 N,3,8,1 N,4,7,1 N,11 N,14,,1 E,1,2,3,4 TYPE,2 REAL,2 E,11,1 ! TYPE 2 ELEMENTS WITH REAL CONSTANT 2 E,14,4 NSEL,S,LOC,X,7 CP,1,UX,ALL ! APPROPRIATE NODAL DISPLACEMENTS COUPLED NSEL,S,NODE,,1,4 CP,2,UZ,ALL NSEL,ALL M,1,UX MODE,1 NSEL,S,LOC,X,8 D,ALL,UX ! APPLY DISPLACEMENT CONSTRAINTS NSEL,S,NODE,,1,4 D,ALL,UY NSEL,S,LOC,X,0 D,ALL,ALL NSEL,ALL FINISH /SOLU SOLVE FINI /POST1 *GET,F2,MODE,1,FREQ *DIM,LABEL,CHAR,1,2 *DIM,VALUE,,1,3 LABEL(1,1) = 'f FLD81 ' LABEL(1,2) = 'Hz' *VFILL,VALUE(1,1),DATA,1.5293 *VFILL,VALUE(1,2),DATA,F2 *VFILL,VALUE(1,3),DATA,ABS(F2/1.5293) /COM /OUT,example_reduced,vrt /COM,------------------- RESULTS COMPARISON ------------- /COM, /COM, | TARGET | ANSYS | RATIO /COM, *VWRITE,LABEL(1,1),LABEL(1,2),VALUE(1,1),VALUE(1,2),VALUE(1,3) (1X,A8,A8,' ',F11.4,' ',F11.4,' ',1F6.3) /COM,---------------------------------------------------------- /OUT FINISH *LIST,example_reduced,vrt
Archive Documentation