Damping and postprocessing in a transient analysis

[SuperAl]

I'm trying to model the response of a simple, steel, BEAM4, framework subject to shock. I have successfully applied a time history of displacement of the four points at which my framework is connected to earth. I have a point mass attached by rigid region to 8 nodes on the framework. I have included the weight per unit length of the beams and applied gravity.

I am using the full transient analysis rather than superposition or the other option. The initial transient result matches a static analysis in terms of reaction forces and bending moments. The ensuing modelled displacement matches my input.

I'm not entirely sure how to view my results to check for stress and strain during the process - I haven't much experience of postprocessing.

I have looked at my reaction forces and 'structural moments' at one of the nodes and all my results look very 'noisy'. I have tried defining some damping using BETAD. I'm not sure how to calculate this - I have used an arbitrary damping ratio of 0.03, since the few example files I've seen use this, and the lowest frequency from a modal analysis ~40Hz. This hardly changes my results.

Can anyone offer any further advice?

Thanks in advance.

 

[Drej]

Check your modal analysis to find the frequency response of your structure. Try finding the two frequency responses that you're interested in and then tune the ALPHAD and BETAD to these frequencies. The two frequencies will be damped exactly to the damping ratio, but this range will be damped and you will see some damping outside/within this. I would also consider using a slightly higher damping ratio of 0.05 (5%) for your structure. This is easily justifiable if you check most codes, but there are always disclaimers for this though, so be careful. Assume you're using /post26 to see your noisy results. This is usually quite normal for a displacement time history. If you change to force this noise will disappear (useless to you, I know, but true!).

How have you calculated the time step, t? Are you following the guidelines in the help? Also, when you say you've calculated BETAD, how exactly have you done this - are you sure your method is correct? It's easy to use the equation for BETAD and not change the units to hz for example.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Drej]

I'd also recommend you take a look at the FFT of your time history if you haven't done so already.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[SuperAl]

Dear Drej,
Thanks for your responses.

My displacement time history is quite simple in that it is close to being a half sine wave of duration 200ms. The sample rate is 1ms but, to save time whilst I sorted out a method, I have been inputting the displacement every 20ms. I have arbitrarily chosen a time step of 5ms for most of my load steps rather than calculate it. I will RTFM(!) again and perhaps reduce my timestep or try auto timestepping (with caution).

I calculated BETAD from the following equation :-
? = 2 ?i/?i
where ?i is (arbitrarily) 0.03 and ?i is 40Hz (the lowest frequency from a modal analysis).
This assumes ALPHAD to be zero since the help manual states "In many practical structural problems, alpha damping (or mass damping) may be ignored (? = 0)".

I did also try quite a large range of completely arbitrary values of BETAD, none of which totally removed the noise.

I could change my input to force rather than displacement but I don't know how I would then restrain the model. My four attachment points are currently restrained in the horizontal plane and I am inputting the vertical restraint. If I inputted a vertical force at these points instead, how could I restrain it?

I don't honestly know what frequency response I'm interested in!!! I obviously know the input frequency - should I be tuning the damping to this frequency?

My ultimate goal is to assess the direct and bending stresses within the framework members. Am I doing the right sort of assessment?

Hope to hear from you soon.

 

[Drej]

In isolation, your Beta damping should be calculated using:

[β]=4[π][ξ]/[ω]

where [ξ] is the damping ratio, [π] is 3.141592.. and [ω] is the frequency in Hertz.

I would recommend, however, that you tune the damping to the first two frequencies (that is unless the two frequencies are miles and miles apart, then it won't matter so much) just to ensure you model realistic structural behaviour. If you do the RTFM thing then there is an excellent explanation in:

Structural Guide> Chapter 5. Transient Dynamic Analysis> 5.10. Other Analysis Details

for both damping and the time step setup.

I don't honestly know what frequency response I'm interested in!!! I obviously know the input frequency - should I be tuning the damping to this frequency?

No. You should tune the damping to the fundamental frequencies of the structure from your modal analysis (usually the first two). I said to you previously that it would be useful to know the frequency content of your time history (by taking an FFT of the data). This is very important since if your input frequency matches the system fundamental frequency then obviously this spells bad news (or just bad luck!). If you know the forcing frequencies then you can design out these in your structure by changing any of the variable which dictate this frequency i.e. using:

[ω]_i=1/2[π](k/m)^0.5

where [ω]_i is the ith frequency in Hz, k is the structural stiffness and m is the mass. You should be interested in the fundamental frequencies because these are the most damaging to your structure. Low frequency = high displacement = high stress; high frequency = low displacement = low stress (relatively speaking). Hence why your damping should be applied to the fundamental modes (damping at high frequencies is pretty irrelevant in most structures, unless the fundamentals are of high frequency of course).

My ultimate goal is to assess the direct and bending stresses within the framework members. Am I doing the right sort of assessment?

I think so. Obviously there are issues with using the correct structural code (ASCE 4-98, ASME etc.) for your industry and/or the application (nuclear/civil, etc.) but this is a pretty straightforward analysis.

Cheers.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com