Regarding modal analysis

Hai,

1) My first concern -Whether stress singularity has any influence on numerical simulation of modal parameters?
2)My second concern- I carried out modal analysis of huge structure with element size say X(somewhat coarse mesh). I founded out the modal parameters(modal frequency and mode shape).

Again I refined the mesh uniformly,that is I meshed the model with element size X/2. The first modal frequency decreased by 400Hz.

Once again I refined the mesh,that is meshed with element size X/4. The first modal frquency decrased compared to the earlier model(Element size=X/2) by 5Hz.
If again I have to refine the mesh it may take huge time.
I feel the moal model is approximately converged.Whether I am right? Whether I have to converge the modal model with zero HZ differnce or I can proceed with the current model itself.
3) The third concern is- I am planning to cross check the numerical modal parameters with the experimental modal parameters. If there is a deviation, I want to correct the numerical modal model.
In this regard,On what basis I have to correct the numerical modal model,so that it will correlate with the experimental one.Whether it is based on modal frequency or FRF? In what way I can redistribute the mass and stiffness of the struture?
Thanks in advance.

Regards,
Vineet

 

[GregLocock]

1) Don't know, probably, I guess it will tend to increase the local stiffness of the structure, hence increase frequencies.

2) 5 Hz error in a 20 Hz mode is very significant. 5 Hz in 400 Hz probably is not. Rule of thumb for a car's body is that 10 mm elements should be OK for modes up to 100 Hz or so.

3) Correlation with the real world? Well done! To get good correlation you have to correlate modeshapes as well as frequencies, these may guide you to look at errors in particular parts of the structure. Is your overall mass correct? How good are your boundary conditions? if you are using rigid elements can you justify using them? Most mistakes I've seen are what I would call 'mechanism' errors ie spotwelds missing, or panels assumed to be able to communicate loads that they can't in practice.

Cheers

Greg Locock

 

[vineet1977]

Hai,

Thanks Greg Locock.

1) I will explore the effect of stress singularity on simpler model.

2)The structure under consideration is having first natural frequency of 750Hz. I think deviation of 5Hz is insignificant.

3)The actual model consists two sheet metal structures welded together.

I will correlate the results with the experimental values of modeshapes and modal frequencies. Whether we can get mode shape description using two channel FFT analyzer.
I thought inorder to get mode shape description in two channel FFT analyzer,we have to do take multiple FRF by varying the position of impact hammer exciter and keeping the accelerometer at the same location(Using reciprocity principle).Whethet I am right?
I planned to carryout the analysis and experiment for FREE-FREE condition priminarily.Once it is correlated,it will be further proceeded with the complex actual boundary conditions.
The model has seam welding of two sheet metal structure.
I represented the weld as beam elements with negligible mass and stiffness of the base material.

Regards,
Vineet
vineet

 

[GregLocock]

re 2) 5 Hz in 750 is fine

You can move the accelerometer and keep the hammer in the same place, or vice versa. A good validation of your experimental technique is to check that you do get reciprocity.

Starting from free-free is a good idea - experimentally is is often difficult to get good idealised boundary conditions.

Your structure sounds very simple - it may have confusing symmetric/antisymmetric modes.

Cheers

Greg Locock

 

[FeaGuru]

As far as the stress singularity goes, I would suspect this would not affect the natural frequency. Only if it is actually connected at this point and has a relatively large displacement at this point will it matter. Otherwise, say if it were a sharp corner, nah, it wont matter, why would it? Its the global stiffness that matters.

As far as testing goes, I dont believe you can just move one and not the other and get good results. I have seen this approach often, but I have a hard time believing it. If the accel is on a node, by moving the hammer around you still cant excite enough energy into the node to get it to move adequately to show up. I ran an analysis one time and the results didnt correlate with the testing. I asked about the testing, retested it, and found that they had the accel at a node and it just wont show up until you move the accel away from the node. Then all of a sudden a mode appears.

 

[GregLocock]

Well, sorry FEAguru, I've run a modal analysis lab for several years, and you are dead wrong. Reciprocity does work on real structures. I typically used to test complete vehicles, and even with all the non-linearities present in real complex structures like that you still have the option of moving the excitation or the accelerometer. For practical reasons when using a shaker you normally move the accelerometer, obviously.

If you apply the excitation at the node then it will see infinite modal mass and you will not be able to get any energy into the system. If you have the accelerometer at a node, then you will not see any response, because it isn't moving.

If reciprocity doesn't work in practice then how could a multishaker excitation setup work?

Cheers

Greg Locock

 

[vineet1977]

Hai,
I have the numerically simulated results before proceeding for experimentation.So, I have complete description of mode shapes. I attached the accelerometer and excitation in the maximum response region(anti-node in modal sense).
I carried out modal analysis of one of the body with free-free condition.The first experimental modal frquency(220Hz)was differing from the computer simulated frequency by 4 hz.
I checked for the first four frquencies,the maximum difference was 30Hz.
But the main problem was only of the FFT analyzer.I feel multi-channel might had been convenient.Due to certain resons I have taken damping values only for the first 3 modes.The damping values is 0.07.The material is cast-iron.
Whether I can use this damping for higher modes also?
Second thing is the FRF values obtained is in terms of acceleration and displacement and the unit is in dB.How to convert this in to actual displacement?

Regards,
Vineet
vineet

 

[GregLocock]

4 Hz on your first mode is great, if the mode shapes agree. Guessing your 4th mode is around 300 -400Hz, 30 Hz error isn't so good, but since you haven't correlated mode shapes yet there will be bigger issues (grin).

0.07 is rather low, if it is %age, for cast iron, or very high if that is an absolute figure. I'd certainly use the experimental value for all your modes if they are all flexural, for example.

Your FRFs are in dB re m/s/s/N ? To convert them into linear units you need to invert the equation dB=20*log(Y1/Yref) where Yref is your reference value for your dB scale, and Y1 is the linear measurement equivalent to the dB. To convert them into displacements you need to integrate twice wrt time, ie divide each FRF bin by (2*pi*freq)^2. This will give you m/N.

When you have done this you will need to look at the phase plots and turn your amplitudes into Real and Imaginary parts. Then you will be able to compare them directly with your calculated mode shapes.

Incidentally it is often a bad idea to mount your shaker at an antinode, really you want to excite as many modes as possible, typically the ends or corners of free-free structures are best, since they are not nodal for any modes.

You are very lucky to be doing both the analysis and the testing yourself, you will learn a lot and this should increase your understanding way beyond that of most node-pushers.
Cheers

Greg Locock