Modal Analysis 2

[Eser]

Hi All!

I have a simple cantilever beam model, that I calculated the natural frequencies and I want to do a mode based steady state dynamic analysis. I want to first apply a load which is a sine function of the frequency. I defined it like that:

*AMPLITUDE, NAME=sinus, DEFINITION=PERIODIC
1,w,0.,0.
0., 1.

From the previuos step we have the first natural frequency is equal to the 14,014 rad/sec and 2.23 Hz. What should I write for the "w" in the previous definition so that I have the frequency of the force equal to the natural frequency of the system so that we have very large magnitude of displacements for an undamped system.

Thanks in advance,

Eser

 

[PamCrash]

Forget the *AMP-card. Try this step after the frequency step

*STEP
*STEADY STATE Dynamics
2.23,
*CLOAD
LOADNODE,LOADDOF,YOURLOAD
*MODAL DAMPING
..
..
*ENDSTEP

BTW, if the damping is zero the vibration magnitude will be infinity.

 

[Eser]

Thanks for your advice but How can I define the force as a sine function without defining *amplitude?

 

[Drej]

If you look at the details (the manuals) of what the poster (Pamcrash) has told you, you'll find that the *STEADY STATE DYNAMICS card is exactly what you're after. This is a forced vibration (harmonic) loading type analysis, the input of which is a steady state harmonic (sinusoidal etc.) load. Don't forget the damping as Pam mentioned.


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

 

[Eser]

I have already used *Steady State Dynamic Option, maybe it is better to represent the rest of my input file so that it becomes clear what I really want to do.

*AMPLITUDE, NAME=sinus, DEFINITION=PERIODIC
1,14,014,0.,0.
0., 1.
************************************************************
*STEP
*STEADY STATE DYNAMICS,FREQUENCY SCALE=LINEAR, INTERVAL=EIGENFREQUENCY
0.0,2000.0 ,20
*CLOAD, AMPLITUDE=Sinus
204,2,1
*MODAL DAMPING, MODAL=DIRECT
1,6,0.05
*SELECT EIGENMODES, GENERATE
1,6,1
*END STEP

If I change it like the way PamCrash explained will I have force of frequency of 2.23 and will it be a sinusoidal function? If I have a more complex Fourier Series function of force then what should I do?
I have some troubles in understandind mode based stead state dynamic type of analysis. Sorry for disturbing you.

 

[PamCrash]

Eser,
understand that the steady state dynamic analysis is a frequency domain analysis. The frequency range of interest (here 0. - 2 kHz) is scanned stepwise and the system is investigated at each frequency step. The load is assumed to be sinusoidal and the magnitude will be taken from the *Amplitude section, which contains the load magnitude vs. frequency.

Pam

 

[Eser]

So what I understand is the force is defined as F=sin(w*f) where w is defined in the previous input file as 14,014 and the f is the frequency. But we have always the high deformations at the natural frequencies no matter how the force defined. Because it only gets the magnitude of the force from the *CLOAD, AMPLITUDE=Sinus but the frequency of the load is taken between 0-2KHz stepwise and when this frequency is equal to the natural frequency we have large magnitude of deformations. What do you think am I correct?

 

[PamCrash]

See example below. A beam with first resonance at 125.23 Hz. An load excitation (amplitude = 1.) is applied in the second step exactly at that eigenfrequency. The force vs. time function here is:

F(t) = 1. * sin(2*Pi*125.23 Hz * t)

1. is the cload amplitude

Hope everything is clear now !



*NODE
1,-2.775558E-16,10.00000,0.000000
2,-2.775558E-16,-5.551115E-17,0.000000
3,10.00000,-5.551115E-17,0.000000
4,20.00000,-5.551115E-17,0.000000
5,30.00000,-5.551115E-17,0.000000
6,40.00000,-5.551115E-17,0.000000
7,50.00000,-5.551115E-17,0.000000
8,50.00000,10.00000,0.000000
9,40.00000,10.00000,0.000000
10,30.00000,10.00000,0.000000
11,20.00000,10.00000,0.000000
12,10.00000,10.00000,0.000000
*ELEMENT,TYPE=S4,ELSET=P1;Default PSHELL Property
1,12,1,2,3
2,11,12,3,4
3,4,5,10,11
4,9,10,5,6
5,6,7,8,9
*SHELL SECTION,ELSET=P1;Default PSHELL Property,MATERIAL=M1;Default MATERIAL
1.000000,
*MATERIAL,NAME=M1;Default MATERIAL
*ELASTIC,TYPE=ISOTROPIC
5000.000,0.4000000
*DENSITY
1.400000E-09,
*STEP,NAME=Anonymous STEP 1
*FREQUENCY,EIGENSOLVER=LANCZOS
3,
*BOUNDARY,TYPE=DISPLACEMENT
2,1,6,0.000000
1,1,6,0.000000
*END STEP
*STEP,NAME=Anonymous STEP 2
*STEADY STATE DYNAMICS
125.2300,
*MODAL DAMPING
1,3,0.5
*SELECT EIGENMODES
1,2,3
*CLOAD
8,3,1.000000
*END STEP

 

[Eser]

Thanks PamCrash it is really clear now. I have only one more question. If we want the force function as for example F=5*sin(2*Pi*2.23Hz*t)+2*cos(2*Pi*13.97Hz*t)+3*sin(2*Pi*24.56Hz*t) then how can we define it in the input file?

 

[PamCrash]

Run *Steadstatedynamics for these three frequencies and superpose the results.

or

Run analysis in time domain. See *ModalDynamics or *Dynamics

Pam