Interpretation of Vonmises stress and displacement results 3

[feaplastic]

Hello Forum Users,

How to interpret the von mises stress and displacement results from normal mode analysis.

I assume,

Normal mode analysis does not give exact displacement value. (Frequency response analysis is required). So, stress output is also not correct.

2. Model: 100*10*1.5 mm. one end is fixed.

Steel Properties: E = 2.1E-5 N/mm2, Nu = 0.3, rho = 7.9E-9 Ton/mm3.

First mode at : 125.59 HZ

stress: 2.64E4 N/mmm2.

Does it mean, when the model will fail in above freq if it is excited to that freq?

Am i missing something? could we consider or should ignore this stress output.

Any help would be nice.

 

[rb1957]

i seriously question your E ... 10^-5 MPa ??

 

[feaplastic]

Sorry rb1957. Just E = 2.1 E5 N/mm2.

 

[rb1957]

my interpretation (and this could easily be wrong !) of the stress is that this is the stress in the structure if it is allowed to resonant at the critical frequency. this stress would not occur in the real strcuture if it was just a transient frequency.

 

[GBor]

Stress results from a modal analysis are meaningless by-products of the way your processor works. It sounds as though your software calculates displacement values and calculates stress from those displacements, which is not uncommon for FEA software. The problem with this process is that the displacements are not true displacements...they are mode shapes designed to indicate how the object would displace if excited by a certain frequency. It's like having the frequency without the amplitude. To get meaningful stresses and displacement, another analysis (like frequency response that you mentioned) is required.

 

[rb1957]

to my mind that poses the question ... why output these numbers ? sounds like the ouptut should be limited to the frequency and the nominal displacements (describing the mode shape).

 

[FEMdude]

rb1957, stress/energy density output is useful in case you want to develop the structure further; ie it tells where to put more material to increase the frequency.

 

[feaplastic]

Gbor,

Thanks. But, do u have any explanation why displacement is not true or why it is not possible to get the true displacement in mode analysis.

FEMdude,

I agree with ur comment in general. But here displacement and stress results are not reliable. Still is it so?

 

[GBor]

feaplastic,

Modal analysis is the simplist form of dynamic analysis. It is performed under a "no load" condition and ignores any system damping. Because of this, you get the tendencies (mode shapes) of an object to deflect, but not the true deflection that it would see under load. You can only determine the true deflection when an actual loading scenario is used (i.e. frequency response). In short, you are calculating eigenvalues and eigenvectors, not displacements to a "real" load.

Analytically, you are solving for non-trivial solutions to an equation of motion: Mx[sub]dd[/sub][sup]2[/sup] + Kx = 0. The solution to this problem does not provide a unique solution of the response. The solution is normalized amplitude ratios.

Hope this makes sense. If not, pick up a vibrations book and see what you can find.

 

[FEMdude]

feaplastic,
displacement and stress values are not realistic, but the shape of the deflection and stress locatios are. So you can estimate where to expect problems due to vibrations (max stress area), or how to make the structure better (put material/stiffness where max energy density is located).

 

[feaplastic]

Thanks FEMdude. You mean to say irrespective of value the problematic location will be same.

You are right. For our original problem, some region were broken during test. When i did the mode analysis for the same component, I got more stress/element strain energy in the same location where it is broken eventhough i did not quantify the value.

GBor, I read one of your reply in the following thread.

thread825-146900.

Now, i have same question. After doing the mode analysis, i have natural frequency. From this, how can i create a input for frequency response analysis to see the real response. I have only Freq. Or simply, what is the load condition for freq response analysis.


Thanks for your help.

(You guys need more than a star, Maybe part of my salary)

 

[GBor]

You have to have either a power spectrum density or acceleration spectrum density...something that defines the amplitude of your forcing function. With the modal analysis, you have the frequency of the forcing function (the sin(wt) portion), now you need the coefficient representing the amplitude. You input the power spectrum density which is generally defined by your system. For instance, some aircraft documents define a table for certain locations within the aircraft similar to the following:

Frequency PSD (g^2/Hz)
20 0.025
40 0.025
50 0.04
500 0.04
2000 0.0025

You input this into the PSD for your software and it checks the natural frequency from your modal analysis, determines the amplitude based on the PSD and applies this to your model, generally at the boundary conditions. From this, deflection and stress can be calculated based on 'real' loads.

 

[hacksaw]

the dynamic analysis is for an arbitrary amplitude, while it is quite useful, it is only the first step in the solution

the next step is sorting out the response to you excitation

 

[meshparts]

Hello,

I found this thread very interesting, but I have a comment on what GBor said:

"Modal analysis is the simplest form of dynamic analysis. It is performed under a "no load" condition and ignores any system damping"

I am sure, GBor meant the undamped modal analysis.

A modal analysis can also be performed with damping. A damped modal analysis would lead to a (2n x 2n) system matrix of the eigenvalue equation, where n is the number of DOF's. Therefore a damped modal analysis would take much more computational time than an undamped modal analysis.

In most cases the systems are light damped and the difference between damped and undamped eigenvalues and eigenmodes are very low. This is the reason why most time undamped modal analysis are performed.

Regards,
Alex

 

[feaplastic]

GBor,

Thanks. Excuse me for late reply. Definitely i do not have any power spectrum density data and even i have no clue how to do it in Nastran.

I extraced normal modes and applied acceleration(15 m/s^2) at a range of freq of 0 to 60 Hz. At resonant freqency looked for displacement and stress. My stress values are in the order of 10^-12 and displacement around 10 mm. Something may be wrong and trying with different loading options like instead of acceleration load, displacement.

Hope my method makes sense. Any further suggestions?...

Thanks for all help.

 

[feaplastic]

Hello,

I ran into another problem. As i said in my previous postm I did a static analysis for cantilerver beam with steel matl, and got displacement(25 mm) and von mises stress at fixed boundary (45 MPa). For the same model, i did the frequency response analysis expecting at 0Hz frequency, displacement and stress values will be same like static analysis. I got same displacement but stress is the order 10^-14, not 45 MPa. Why it is so. Could you please explain.

Thanks for any help.

 

[GBor]

You have generated what appears to be a fictitious acceleration spectrum density. The results on a graph would be a horizontal line, but may not have real meaning.

As for the difference between your static and dynamic analyses, 0Hz doesn't make analytical sense. The fundamental theoretical basis of this thought is out of hte realm of the governing constituitive laws...that's a fancy way of saying 0Hz doesn't equal "static".

Check out this site:

http://femci.gsfc.nasa.gov/random/

I like the way this information is presented, and if you have a reasonably strong math background, you can probably understand why you are getting some of the answers that you are seeing.

 

[feaplastic]

Interesting Gbor. I did the same analysis in Hypermesh and i got what i expected(same disp and stress as static results).

Another user did the same with patron and nastran and got the same. So i thought it is a problem with Hypermesh and Nastran interface.

Now, you have a different opinion(it wont be same). I check out the link. Anyway i am not so good in Math. Other users, any other thoughts?

Happy Holidays.

 

[GBor]

Well, looks like I need to go do the math. My opinion that they wouldn't be the same was more of a quick reaction...not a lot of thought put into it. Guess I'll have to think about it since it worked in Hypermesh.