Animating Static and Eigenvalue (Modal) Analyses

Animating Static and Eigenvalue (Modal) Analyses

Recent versions of Ansys LS-DYNA incorporate the implicit solver, and this means that they can generate eigenvalue results. In addition it is possible to post-process static, eigenvalue and other solution sequences from Nastran analyses (see APPENDIX F).

Analyses of these types differ from conventional transient analyses in that each "state" is assumed to be:

• Eigenvalue analysis: A given modeshape


• Static analysis:The result of a given static loadcase combination.

Therefore when such analyses are animated it does not make sense to animate over states, rather a given "state" is cycled through a sinewave function to produce a "modeshape" plot.

This has two implications for animation:

ANIM >, SET_FRAMES Setting the number of frames that are to occupy 360 of the sine wave By default each 360 degree cycle of animation is split into 11 frames, which actually means 22 images, since the +ve and -ve cycles are symmetrical about their respective peak values. The SET_FRAMES command in the ANIM > popup menu (which replaces the SET_STATES command in this context) allows you to choose a different number. More frames will give a smoother but slower animation. The Custom... option permits any number of frames to be defined, and also defines the period for the sine wave. Normally the MAX->MIN option will be used, as this reflects the states internally to generate a 360 0 animation from 180 0 of frames. The MAX->MIN->MAX option is only required when generating files for an external viewer that is not capable of "reflecting" a 180 0 sequence into a 360 0 one. It looks stupid on the screen, but will duplicate the frames to produce a full 360 0 sequence in the file.

The frames slider cycles through the 0 - 360 cycle of frames, not through states

The frames slider, and other controls, cycle through the modeshape phase angle, not states. (See Basic animation controls)

Factors on results when animated by "modeshape"

It is intuitively obvious that the factors on displacement to produce modeshapes need to be both +ve and -ve [factor = cos(time)]. It is less obvious what the factors on the corresponding results should be: magnitude values (such as von Mises stress) need a +ve/+ve, whereas direct stress tensor components (such a X direct stress) should be +ve/-ve, and components such as thickness should not vary at all.

Thus factors on data components through the 0 - 360deg vary as follows:

+ve/-ve factors, f = cos(theta)	+ve/+ve factors, f = |cos(theta) |	Unity factors, f = 1.0
[Sx,Sy,Sz,Txy,Tyz,Tzx] stress tensor [Ex,Ey,Ez,Exy,Eyz,Ezx] strain tensor Shell force & moment resultants [<outer fibre>] derived stresses [X,Y,Z] displacements	Everything not in the other two columns.	Thickness Shell Area Volume Outward normal Basic [X,Y,Z] coordinates Current [X,Y,Z] coordinates