What amplitude is used for a finite element modal analysis excitation?

In a typical finite elements analysis package, a modal analysis gives the N first natural modes, and it is possible to get the equivalent stress and total deformations for each of these frequencies.

But what amplitude did the solver use to get these results?

Why can't we obtain a gain instead, for displacements and stresses and for each frequency?

• Does the analysis package not have a "default" spectrum that is used? Or maybe a user-specified one? – hazzey Apr 17 '15 at 19:30
• Thanks for the comment. Spectrum? I would expect the amplitude of the excitation to be constant for each frequency for the results to make sense!? It may be defined somewhere, but I haven't found it so I was thinking that maybe it was a conventional thing (like 1m of amplitude regardless of the frequency). I'm using ANSYS R15 if that makes a difference. – Mister Mystère Apr 17 '15 at 20:23
• Do you not have loads defined for the analysis? – Trevor Archibald Apr 17 '15 at 21:31
• I have constraints, not loads. None of tutorials I've seen (I was starting to have doubts) defined any; that's the trouble about oversimplified software: no idea about what's used by default! – Mister Mystère Apr 18 '15 at 2:59

2 Answers

The short answer is, there is no amplitude used. Even more important though, is the fact that the displacements and stresses shown in the results of a modal analysis cannot be used to say anything about the physical behavior of the part in absolute terms.

The basic equation of motion is

$$[M][\ddot{U}]+[B][\dot{U}]+[K][U]=F(t)$$

$M$, $B$,and $K$ are matrices for mass, dampening, and stiffness, respectively, and $U$ is the displacement. The material properties are known, and we are solving for the displacement. These are specified for the individual nodes created when meshing an FEA model. For a modal analysis, we ignore the damping effects, and assume there are no loads present. This essentially poses the question "If we constrain the part in a certain manner but apply no load to it, what are the possible ways in which it will vibrate?"

Look at the equation of motion when we neglect the damping and apply no load (F=0)

$$[M][\ddot{U}]+[K][U]=0$$

We are trying to solve this equation for non-zero values of $U$; that is, points at which the inertial forces and spring forces of the material are equal. In this idealized case of no damping, the part could theoretically vibrate through these points forever after an initial displacement/force is applied.

In solving the idealized equation above, we also let

$$[\ddot{U}]=\lambda[U]$$

where $\lambda$ is an eigenvalue. This is a consequence of harmonic motion, which makes sense when you think about it a bit. If a part is oscillating between two positions and the points of the part take linear paths between their two positions, the acceleration vector will always be a linear multiple of the displacement vector.

In the final form of the equation, we see that we only have 4 distinct terms:

$$\lambda[M][U]+[K][U]=0$$

Since $M$ and $K$ are known, we're just looking for a displacement matrix for which a constant $\lambda$ exists. But given the nature of this equation, it's easy to see that for a matrix $[V]=A[U]$ where $A$ is an arbitrary constant, $\lambda_U=\lambda_V$.

Lastly, it's useful to note that the units of $\lambda$ are $s^{-2}$, meaning that $\lambda=\phi^2$ with $\phi$ being the resonant frequency of the vibration mode in question.

So as I said at the top, there is no amplitude used to the actual main calculations in a modal analysis. To display the results and give the "displacement" values in the results, there is some standard amplitude or normalization done, but those numbers are not what you're looking for in a modal analysis, and they shouldn't be used in absolute form; how you can use them is in determining the proportionality of displacements between nodes. If you see point A has a displacement of 2mm when point B has a displacement of 1mm, you know that 2:1 ratio will always exist for this vibration mode.

To determine how much a part will actually vibrate, you have to do a full vibrational analysis, defining the loads and their frequencies yourself, using the knowledge you've gained from the modal analysis.

Two good references:

The amplitudes of the modes from a vibration analysis are arbitrary. Often they are "mass-normalized" which is mathematically convenient for using them in a subsequent step in the analysis. There may be an option to scale the in other ways, for example "engineer's normalization" where the largest deflection is set to 1.0, or the option to scale a specified degree of freedom or stress component to any amplitude you choose.

You may know the amplitude of vibration by testing the structure, or by monitoring it in use with strain gauges or accelerometers. If so you can scale the analysis results to match what you know.

If you want to calculate the actual amplitudes and stresses for a given set of loads, you need to do a steady state response analysis, and/or a transient response analysis, whichever is appropriate to the loading and operating conditions.

• I concur with your answer. I know Abaqus, for example, provides results normalized to mass by default and displacement if desired. For a mass oscillating at its natural frequency (undamped) the response is unbounded for any ampltide of excitation. – a_hipster_peter_pan Apr 27 '15 at 1:09