This is an announcement---a complaint if you will---maybe it will help someone who gets confused.

The so called "frequency" analysis has the purpose of finding the natural frequencies and mode shapes of your meshed body. This analysis is akin to finding the frequencies of a vibrating string, or, slightly more sophisticated, that of beams (which is related to column buckling). The results are (by default) shown as "resultant displacement" with real units.

**Let it be made clear** that it is impossible to calculate actual displacements with such analysis. It only gives you the frequency at which the mode occurs, and the shape of the mode. The actual displacements depend on the input excitation, as has been said previously in other posts. In a theoretically frictionless/dampingless world the displacements would be infinite, because by definition, these are the resonant frequencies of your system and all excitation at that frequency gets amplified. By this very fact, under random vibration, the system tends toward these frequencies. Moreover, the only two material properties that matter in this calculation is the Young's modulus and density.

So, Solidworks, shame on you for:

1. Putting real units on the scale bar of these plots.

2. Making the magnitudes completely absurd---I'm getting 3 meters of displacement on a structure not 1 meter tall.

For those of us who know this is nonsense, it can almost be ignored. But it inevitably means extra phone calls and raised eyebrows come design review time. You cannot expect your customers to first give a short lesson on the subject to their clients.

No one yet has responded that you can turn off the colors (see pic). That's what I do. Personally I think it makes the results easier to understand for everyone. What I would prefer more (as a user) is to have the ability to change the software's preset defaults to

mydefault settings to have this behavior.Some other examples where I would like to see the settings in Simulation customizable:

(a) I always like to make my mesh control ratio 1.25 and there is no way to change it from the 1.50 value set by the software.

(b) Different number formats for each type of result, like: strain in scientific; stresses with fixed one decimal place; and displacements with engineering notation (E+03, E+06, ...).

## Attachments

I feel that many people who is posting here do not have minimum knowledge of FEA.

No software will give Displacement in Natural frequency analysis.

It is the duty of Analyst to explain to the customer baout the Analysis.

To get the displacments and stress there are other modules such as Dynamic analysis-time history analysis, random analysis, hormonic analysis.

Frequency analysis- names itself says that it is for frequency not for any other outputs.

Frequency analysis is the starting point for dynamic analysis. Based on the results one will decide.

For your information All softwares in the world available for analysis (Ansys,Nastran.........) will show legend either in units' m' or 'mm'.

There is no need to feel shame for solidworks as this is followed in all analysis packages.

If you are referring to displacement shown by natural frequency study, you are correct that the values are meaningless and could not be calculated without an excitation input. The plots are valuable for showing the mode shape of deflection at the resonant frequencies.

Quickly finding the natural frequencies and mode shapes is an excellent first step in analysis sequence.

On the contrary, displacement plots have meaning and are not senseless. All FEA codes do this with natural frequency and mode shape extraction, and it is mearly a scaling of the eigenvectors that is being done: an arbritray value is selected to normalized the scale. The equilibrium equation that is being solved has no external forces. Recall: F = MA + CV + KU. "F" (external forces) is set to zero, and "C" (damping) is set to zero, so the equation is 0= MA +KU. For a one-dimensional analogy, if you assume a vibratory solution to this differential equation such as U(t) = A*sin(wt), you can plug it into the equilibrium equation and see that it works (try it). When you solve it, the "A" cancels-out (if assumed non-zero), and the solution is w = SQRT(K/M). The "w" is the natural frequency. Right-off-the-bat, the amplitude "A" can have any value and the proposed solution will always satisify the equilibrium equation. In a matrix calculation, the U becomes a vector of displacements of every single node in the model, and the "w" term (omega, natural frequency) is indexed for the different natural frequencies for which you have requested extraction. The "U" for each frequency is known as an eigenvector, and the "w" are known as the eigenvalue set, and they are paired as when you request a displacement plot.

The upshot is this: If red-colored areas correspond to "100" (in whatever units), on the legend, and green-colored areas correspond to "50", this means if the structure vibrates at that frequency (which may be excitation of some means without regard to amplitude of the excitation), then you can conclude red-colored areas will move twice as far as green-colored areas, no matter what the excitation amplitude. You can scale other colors appropriately to determine relative displacements in other areas of the structure. Hope this helps explain (at least a little) what is going on in the arithmetic of the code.

Thanks for the insight Anthony! I hadn't realized that's how it was being done.

Although the Plot does represent relative displacements, I still think a quantitative input stimulus is necessary to calculate actual deflection, no?

Anthony---good discussion. The legend of the plot should be zero to 1, or zero to 100, whatever, and certainly not be labeled as millimeters. Fine---if they don't want to normalize to 100 or 1, at least they could remove the units, and call it something other than "URES".

This is now an enhancement request, since my VAR says Solidworks had nothing to say on the issue. Look for it in the 2025 version.