Applying sinusoidal loading

[maheshh]

Hi all,

I have a non linear model (contact elements) and have already solved the static scenario for the assembly. It converges well.

Now I want to subject the same assembly, with the same loading as in the static analysis, to a following transient load:
half-sine wave
10 milli sec. duration
25G peak amplitude

I guess I have to do a transient - full analysis to capture the non-linearity in the model. But I am not able to understand how to apply the loading in this case. Any help would be appreciated.

Thanks.

 

[cbrn]

Hi,
1) TRANS is the only analysis type where full-nonlinearities are taken into account, so you're right when you say it's your only option in this case.
2) you have to apply loads using TABLES instead of fixed values. In the tables, the independent value is TIME and the dependent one is the BC you need. As you need to apply a sine, you can use Function Editor to define this function, then save it to file, then re-import it into a destination table.
3) In TRANS you can not apply an accel to the "grounded" nodes (manipulating the global ACCEL is not the same). You will have to calculate the displacement amplitude that gives the accel value (as you have only one freq and not a spectral distrib, it's only a metter of integration). Look in this forum for other threads that better explain this matter.
4) I think you'd better first run a modal analysis in order to see which are the most crucial frequencies for the system: if your excitation freq is not near some natural one, most probably it will be "damped out" by the system and so the entire time-consuming transient analysis could be avoided. Of course the modal will not have non-lin, but the freq shift they can introduce is generally modest. Moreover, the modal can help you decide how small a timestep to use and how long the analysis should last in order to capture the response of the system.

Regards

 

[maheshh]

Thanks for the response. Following is what I did -

1) This is the table that summarizes my loading condition on a face as pressure. left col. is time, right is pres. I applied this BC on the face.
0 0
0.000833333 4.152983301
0.001666667 8.022721081
0.0025 11.34528599
0.003333333 13.89406945
0.004166667 15.49523702
0.005 16.03958444
0.005833333 15.48998562
0.006666667 13.8839248
0.0075 11.33094
0.008333333 8.005152181
0.009166667 4.133389741
0.01 -0.020281881

2) I also turned the acceleration on.

3) Then in the transient solution control, I set the end time of the run to be 0.01sec, and increment to be 0.000833333 so that there are loading condition corresponding to the time step in the above table.

4) Then I ran the transient analysis (which took a mighty 7 hours on a 4 processor workstation).

Now to post processing:
1) If you look at the table, I have max. pressure exactly mid way, and I would expect my deflection to by maximum at that time step. BUT THAT IS NOT THE CASE
I read in that substep, and then the last substep, the deflection is higher in last substep when the pressure is close to 0.

-------

I cannot understand the 3rd point that you mention above. When you say I cannot apply accel. to grounded nodes, what does that mean? I turned accln. on. Will it not account for inertia forces when i just turn it on. Why do I have to calculate the accleration value based on displacement?

Also, my variable of interest after the run is maximum displacement/deflection of the entire assembly, so how can I use that to calculate accln.?

Thanks.

 

[cbrn]

Hi,
1) sorry, I misunderstood what you were trying to do. I thought that the structure would be loaded somehow and restrained "somewhere" (i.e. that these nodes would have imposed displacements 0 for all DOF), and that you had to "shake" the structure by imposing transient displacement values to these nodes.
If it's the pressure load which varies, then what you did seems perfectly correct from your description.
Only point: you don't need to worry about matching btw timesteps and table steps, because by definition "tables" are special arrays in which the program can interpolate between the values.

2) If everything in the analysis is set up correctly as it seems, I can explain the timeshift btw max load and max deflection only by inertial effects. Your load's frequency is probably sufficiently near to some natural ones of the system, so that there is a response to the excitation and the response is out-of-phase by an amount you can appreciate from your results.

3) To clear this out, I'd suggest to run the same analysis but with 5 - 10 periods of the exctitation (and of course increase the timestep, otherwise it would take 70 hours !...).

Regards