Large deformation in modal analysis

[Mohamed_Wael]

Hi all,
I have been simulating the following rhombus compliant mechanism using Ansys Modal analysis to have a quick understanding about its mode shapes,,,, the problem is that the deformation is extremely large you can see this as the scale is (*10^-5 ) . This result is for sure unrealistic but what does it indicate or what might be my mistake in the modeling https://goo.gl/WbQcxJ

 

[Mech_Engineer]

Hi Mohamed,

As a general rule I would pay attention to the mode shapes and frequencies but ignore the deformation values in a modal FEA analysis. The amplitude of the individual modes is a mass-normalized value which doesn't typically allow for apples-to-apples comparisons between nodes. See here:

https://www.physicsforums.com/threads/ansys-modal-what-does-the-deflection-result-represent.728097/

The simple-minded answer is, you can only compare the relative deflections at different points in the same mode shape. You can't compare the size of the deflections at the same point in two different modes - unless the deflection is zero at that point in one of the modes.

The less-simple-minded answer is, it depends how the different mode shapes are "normalized" when they are output. There are two "common sense" methods that are sometimes used:

1. Make the biggest deflection in each mode = 1.0 (wherever it occurs, usually at a different place in each mode)
2. Make the deflection at a place that you specify in the input = 1.0, for all the modes. (The deflection at other places in the structure maybe bigger than 1, of course).

But more likely, the mode shapes will be "mass normalized", which means the product $x^TMx = 1$ where $x$ is the mode shape vector and $M$ is the mass matrix of the structure. That means the internal energy (potential + kinetic) in different modes is proportional to the frequency squared, for the values of the displacements that are output.

The reason for this choice is because it is very convenient for using the mode shapes as generalized coordinates (in the sense of Lagrangian mechanics) for dynamic analysis both in the time domain (transient dynamics analysis) and the frequency domain (steady state response analysis). Most course notes / web sites / textbooks on dynamics of multi degree of freedom (MDOF) systems will have some of the math behind this, for "simple" systems modeled by point masses connected by springs. The basic ideas are exactly the same for finite element models - the only difference is that the finite element mass and stiffness are formulated in a more general way.