Modal Analysis Appendix Five

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-2 Basics of Free Vibration Analysis A free vibration analysis (a.k.a. modal or normal modes analysis) is performed to obtain the natural frequencies and mode shapes of a structure –Free Vibration analysis does not consider the response of the structure under dynamic loads but just solves for the natural frequencies. A free vibration analysis is usually the first step before solving more complicated dynamic problems. A free vibration analysis is a subset of the general equation of motion:

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-3 Basics of Free Vibration Analysis In free vibration analysis, the structure is assumed to be linear, so the response is assumed to be harmonic: where  i is the mode shape (eigenvector) and  i is the natural circular frequency for mode i. By substituting this value in the earlier equation, the following is obtained: Noting that the solution  i =0 is trivial,  i is solved for:

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-4 … Requesting Results The corresponding ANSYS commands for the Frequency Finder branch are as follows: –If Frequency Finder branch is present, ANTYPE,MODAL is set –The number of modes is set with the nmodes argument, and the beginning and ending search frequencies are specified with freqb and freqe of the MODOPT,,nmodes,freqb,freqe command –All modes are expanded via the MXPAND command. To save disk space and calculation times, the element solution option of MXPAND is not turned on unless stress or strain results are requested.

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-5 … Solution Options For a regular modal analysis, none of the solution options except for “Solver Type” have much effect –“Large Deflection” and “Weak Springs” are meant for static analysis cases and should not be changed. –“Solver Type” can be set to “Direct” or “Iterative” “Program Controlled” or “Direct” result in the Block Lanczos eigenvalue extraction method with the sparse direct equation solver (MODOPT,LANB and EQSLV,SPARSE). This is the most robust eigensolver, as it handles small & large models and beam, shell, or solid meshes, so it is the default option. “Iterative” results in the PowerDynamics solution method, which is a combination of the subspace eigenvalue extraction method with the PCG equation solver (MODOPT,SUBSP and EQSLV,PCG). The PowerDynamics eigensolver can be efficient for large models of solid elements, when requesting only a few modes.

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-6 … Prestressed Modal Analysis For prestressed modal analysis, Simulation performs the two necessary iterations internally: –A linear static analysis with PSTRES,ON is run –A modal analysis is then run right afterwards with PSTRES,ON to consider prestress effects

Training Manual General Preprocessing Procedure March 29, 2005 Inventory # A5-7 … Prestressed Modal Analysis Other items useful for ANSYS users to keep in mind: –No large-deflection prestress effects are currently supported in Simulation, so enabling the “Large Deflection: On” in the Solution branch is not permitted. –The equation solver for the static analysis and the eigensolver for the modal analysis currently cannot be independently set. Both will be affected by the “Solver Type” setting in the Solution branch. –If a Point Mass is present, rigid-body modes may be introduced in a prestressed modal analysis. This is due to the fact that the RBE3-type of surface constraint defined with CONTA174 and TARGE170 introduce 6 DOF but the MASS21 element has no rotary inertial terms (3 DOF). The user can usually ignore these rigid-body modes, as they are associated with the MASS21 elements (verify by checking displacement scale of these mode shapes). No such problems exist for a regular modal with Point Masses.