Which is the right way of considering damping in Response Dynamics?Modal Damp or Material Damping? 2

[ninjaz]

I am trying to validate the strength of the component which operates in a certain frequency range. NX Advanced simulation - SOl 103 Response Dynamics is used to do the simulation. Based on the Mode shapes, I am creating the Frequency Response Event. Now the doubt is, where should I input the damping. The component is made of cast-iron and I would like to give 3% damping.

Following are the two ways, the software allows to feed damping . But which is the correct way?
One for the Mode shape - (Modal Damping)

And other at Material Properties Table : Structural Damping.

Which is the correct way?

 

[karachun]

In Nastran strucutural damping coef. G = 2*dzetta, where dzetta is damping coef, used in dynamics theory.
You can assume dzetta=0,02...0,03, so G=0,04...0,06.

 

[Erik Panos Kostson]

It depends.

If you know the material damping, then of course add it to the material properties (GE) as you showed in your picture (some software will calculate an effective modal damping in the background, based on the material damping properties). Say for instance we have a steel structure on soil, with steel having 2% material damping, and the soil having 10% material damping. If a mode has predominant motion in the steel, then the modal damping for that mode is calculated close to the 2 % (and the other way around, if it is soil based motion then modal damping is close to 10% in this case). In reality it might be in between in this example if the motion is taking place in both parts (soil and steel).

Now if you do not know the material damping, and you have perhaps done measurements (modal analysis) and measured the modal damping for your structure, then it is of course easier to input the modal damping directly.

In both cases we will end up with modal damping because that will allow the modal transformed equation that are solved to be decoupled, and we can then solve single degree of freedom equations for each frequency, mode, modal damping (something that is quite convenient).

Also structure need/should be designed away from resonance and in that case damping is not controlling the motion (damping has an influence close and at resonance). If we are say way below the first resonance, then the structure might be stiffness controlled (vibration amplitude is influenced by the stiffness and not by the damping then).

Hope this helps you to understand the differences.

 

[ninjaz]

That was a good explanation. Thank you. Erik Panos Kostson

And , Now I understand that we should give any one damping , Either Modal or Material. Is it Correct?
Suppose , The mode shape is due to Steel component fixed on a rigid structure. Now I have both Material Damping Coeef,GE=0.03 and Modal damping to be considered as 4% . Now Should I input both values or either one.

FYI: The natural frequency falls little closer to resonance range.

 

[Erik Panos Kostson]

That is OK.

I will assume that you do not have any modal tests where modal damping has been measured, so in this case if you have the material damping (e.g., 0.25%-1%) for cast steel alone (no welds no bolts no connections ...) then enter the material damping coefficient GE only (not both).

If I am wrong and you have measured data and obtained modal damping from exp. modal analysis, then input the modal damping directly only (not both).

In any case you can check that you get the actual damping by doing a harmonic excitation study sweeping a harmonic force over frequency. In this case you can plot your frequency response as shown below (e.g., velocity/Force), over frequency and from that you can get the damping via, damping (%) = (f2-f1)/(f2+f1). This should match whatever you put in to the software.

Also try to move the natural frequency of your part away from the external loads excitation frequency, so not to rely on damping in order to get an acceptable structural response.