Learning Forum

[murali]

Hello,

I am trying to find the response of a cantilever beam subject to an initial displacement. Due to some reason, i am not getting the final results. There is no additional load acting on the beam. Just  the initial displacement with initial velocity zero.  Kindly help.

[Erik Kostson]

Hi

See how to use base excitation with modal super position.

https://www.youtube.com/watch?v=EY5J1jd1EMk

 

All the best

 

[murali]

Hi, Thanks for the link. I still have few doubts, can a displacement initial condition be considered equivalent to base excitation?? 

Just to make my problem clear:

I need to find the transient response of a cantilever beam subject to a transverse initial displacement. The initial vel is zero. There is no force applied, only the initial displacement. But when I do the analysis I am not getting the result.  I need to know how to introduce an initial condition. If it is not possible to get a solution without introducinga force, how do i do the simulation accurately?

[Erik Kostson]

Hi

Can you explain what you mean with initial displacement - how does the function vs time look like?

All the best

Erik

[murali]

 

I meant, just lifting the free end of the beam to, say a few mm, and then releasing it, so that it vibrates for a few seconds and comes back to rest. A typical damped vibration condition.

 

[Erik Kostson]

 

 

Hi

Use full transient analysis instead of mode sup.

You can then use a 2 step analysis .

1st step: lift tip up

2nd step: release (by deactivate at this step - see here : /forum/forums/topic/disable-constraints-in-a-load-step/)

All the best

Erik

 

 

[murali]

 

Dear Erik,

Thanks a lot. I will try this.

Murali

[Erik Kostson]

Hi

That works so you can do what you need.

All the best

Erik

[murali]

 

 

Hi Erik,

Now i am getting the solution, however not accurate. I am supposed to get the second figure, but I am getting the first one. As I alter the step control in analysis setting, the solution changes everytime. Where can I find how to properly give time steps in transient analysis? 

 

 

[Erik Kostson]

 

 

 

 

 

Hi

So you need to have at least 10 time steps in one period to capture a free vibration. Ideally 20 steps per period.

So say the free vibration of interest is 10Hz, or T_period=0.1 s, then the time step in the analysis settings should be T/10 = 0.01 s at least or even better T/20 = 0.005 s (at least for the 2nd step when the free vibration occurs).

See here for more info (3 min.30 s mark – 6 minute mark in the below – time step discussion):

https://www.youtube.com/watch?v=DnfGaJgbXcw

 

All the best

Erik

 

 

 

 

 

[murali]

Hi Erik,

The fundamental frequency is 12.4 hz as per modal analysis. So how many time steps should I use? How do I decide the step end time in each step? Should the auto time stepping and time integration be on for all the steps?

 

[Erik Kostson]

 

 

 

 

Hi

Please see the transient courses for instance the one I sent and try and understand that.

Also make sure you understand the difference between Steps (You have 2 steps), and time step (which is dt in the time integration used of the equations of motion – I showed above how to determine that time step size ~ T_period/10).  You can search this online and get lots of help that way.

The end time for step 1 could be say 1 s (does not matter since 1st step it is quasi-static movement of the tip up), and the 2nd dynamic step could be say 10 * T_period (T_per.=1/freq., freq.=12 Hz for you) so you want to see 10 periods of vibration say or more perhaps say 100*T_per., thus the end of that 2nd step is =
end of first step (say 1s) + 10*T_per. 

Leave also time integration on for both steps (makes steps dynamic so considering mass, damping and stiffness matrix so full dynamics equations of motion 

Also the help manual contains info on the theory of transient dynamics.

So go through material on transient dynamics and linear dynamics.

All the best of luck.

Erik

 

 

 

 

 

[peteroznewman]

Good discussion!

[murali]

Thank a  lot for the help. Finally I have figured out to do it. The animation of deformation is but somehow distorted, although the displacement values in the plot are correct. Why is it so?

 

[Erik Kostson]

Hi

It is because of the deformation scale factor/menu - search for that for more info.

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v232/en/wb_sim/ds_Context_Toolbar.html%23ds_Context_Toolbar

If you are not able to open the links, refer to this forum discussion: How to access the ANSYS Online Help

Guidelines for Posting on Ansys Learning Forum

Hope that helps

 

Erik

[murali]

Hello Erik and  Peter,

Thanks a lot for the detailed explanation. The effort is much appreciated.

Murali

[Erik Kostson]

Happy to help - closing this discussion as it might be useful for others that do similar analysis - if you have any other questions, please open up a new discussion.

Thank you

Erik