what is "Normalising mode shapes" in modal analysis? 2

[fellowmate]

Hi everyone,

I am trying to do the modal analysis of a 3-d cantilever in ansys in order to study the natural frequencies, the amplitudes and vonmisses stresses.I have attempted the block-Lanczo's mode extraction method and obtained the natural frequencies of the first five modes of oscillation,but I have not been able to interpret the vonmisses stresses and amplitudes obtained.Infact I have noticed that an option of "normalised mode shape to" pops up soon after in analysis options for block-laczos showing either "mass matrix" or "unity" options.The stress values are too high and dont seem correct to me,and the amplitudes in "unity" option is almost 1 for all modes while the normalised mode shapes to mass matrix gives very large values of amplitudes.Please help me in this regard.

Thanks and regards
Rajib

 

[GregLocock]

In a normal modes analysis the scaling of the eigenvector is essentially arbitrary. There are at least three schemes I have heard of, max amplitude=1, unit modal mass, and another one I've forgotten.

In a normal modes analysis the physical modal scaling is done by the parameter table, which typically gives a damping value and a real world scaling factor, and a phase for one reference and response coordinate, for each eigenvalue. The real world scaling factor will vary depending on which scaling method was used for the eigenvector.

I'm sure this is all explained in Ewins.

http://www.amazon.com/exec/obidos/ASIN/0863802184/104-0222329-5929574

Cheers

Greg Locock

 

[MikeyP]

It's a guess as "unity" and "mass matrix" are quite ambiguous terms, but here is what I think:

"unity" scaling is probably what is called "unity maximum displacement" scaling. Each displacement value in a particular mode shape is scaled so that the maximum displacement is 1. i.e. you simply divide each value in the mode shape by the maximum value in the mode shape.

"mass matrix" scaling is probably "unity modal mass" scaling. This multiplies each displacement value in a particular mode shape so that the modal mass for that mode has a value of 1.

I wouldn't have thought that either of these would affect stress values. Do the stress values change depending on which option you suggest.

For a cantilever beam, the unity maximum scaled mode shape for the first mode should be increasing values from 0 at the nodes at the root to 1 at the nodes at the tip.

M

--
Dr Michael F Platten

 

[fellowmate]

Hi,

I thank you for your valuable replies.But I dont yet understand how to find out the true values of von-misses stresses and amplitudes? For the first mode of vibration the obtained misses-stress(max)values and amplitudes are as follows:

Unity(displacement) ------ Mass Matrix option

Misses(max)- 0.101 E13 ------ 0.771 E16
Amplitude- 1.005 ------ 7701

The amplitude is too large for mass matrix,since the used cantilever is in micron-dimensions (though the units entered are in SI in ansys).

Is there any method to relate the true values of displacement, stresses and obtained values ?
Because neither value of stress seems right if the units are in pascals.

Thanks and regards
Rajib

 

[franck]

Hi fellowmate,

In order to get stress levels or displacements that make sense, you need to apply an excitation to your beam with some kind of damping.

Franck

 

[elogesh]

Hai,

Franck is already responded to your e-mail.

Modal analysis is for determining the mode shapes and modal frequencies.It is obvious that loads not required for modal analysis.

If your interested in determining the stress and amplitude due to excitation, then harmonic(frequency domain) or transient analysis(Time domain) will do.

Regards,
Logesh.E

 

[izax1]

fellowmate,

Franck gave you the clue.

You will see that you have not defined any dynamic loads to your analysis. At least, that is no required for doing a normal modes analysis. Normalising will just give you options for showing your eigenvectors. Absolute Stresses and displacements are not an option in normal modes. Just relative values.

Bernt

 

[desimontreal]

Interesting forum. I would have thought the results would be meaningless unless you related it to an actual experimental data.

When we do blade vibration test we can scale the normalize modal stress result to actual results to determine the maximum stress on the structure for a particular mode shape and natural frequency. Of course we use stain gauges on the structure at a desired location. Once scaled the results would give us the stresses of the entire structure. Again that is because we initially have no idea of structural damping and the amplitude of excitation is not exactly known. The response of the excitation would depend of proximity to a natural frequency... but I am not an expert.

Des

 

[xydrex]

You cannot interpret absolute values of stresses or any other variables for that matter from mode-extraction procedures. It is purely to see what shape the structure will tend to attain if stimulated at that frequency. Thus the values are relative values of one part of the structure to another. So if you see 100MPa in one region and 200MPa in another, the only info you can get from this is that the former region will be stressed 1/2 as much as the latter w.r.t the contribution from this particular mode. Actual values depend on loading by using steps mentioned by previous people. Also any given loading situation will have contribution from many modes simultaneously. The contribution from the various modes are combined by linear
superposition - so also remeber that you must remain within the linear range for valid results.

 

[izax1]

To get back to the original post, I think it is important to state that natural frequency is a "theoretical" value. It is not possible to find (measure) the natural frequency of a structure the way you find (calculate) the natural frequency in a FE-analysis. A natural frequency will be the sqrt of stiffness divided by mass. So you are able to calculate this without any external loading applied. In reality, that is not possible. So in a real life test, you will get real values for stress, accelerations etc. In theoretical calculations (i.e. FE) you will not. It is just a way ( and a very convinient one) to find frequencies and mode shapes.

 

[xydrex]

You can actually simulate a real mode test in FEA for e.g. shaker excitation and get motion response directly from the nodes. If you input the loads that you would actually use in reality, values of stresses & all else should be very similar. However you would need to use a general dynamic step, which uses direct integration. This is very computationally expensive because it can also handle non-linearities, which is not necessary. Frequency extraction steps are used because its a linear perturbation step, since most vibration problems are in linear range. Stresses you get from this are not absolute. Results of this can then be used to synthesize overall response from operating loads by various modal dynamic step procedures, also linear. These will give operating stresses. To be accurate, do experimental modal analysis to get damping parameter (which cannot be obtained from FEA) and input it into the model.