Inputing acceleration data to ANSYS, Seismic analysis 3

[12civil34]

Hi,

I am modeling a structural component in ANSYS, its reinforced concrete and i've used solid65 as my element with smeared rebars.

I have a ground motion timehistory ( acceleration) that should be applied to the base of the structure (base excitation), my ANSYS version is 12.0.1.

1. Is that correct to input the ground motion using the D ACCL command?
How should I apply the BC?

2. I have introduced structural density for my material. I don't know how to apply the gravity force (due to the mass of structure) in ANSYS? Shal I do a seperate analysis for it? How I should do that anlysis? Do I need to define a mass element for this purpose?

Thanks,
Al

 

[TERIO]

I don't think you can directly apply a base acceleration in ANSYS. I think you may need to integrate it twice and apply it as displacement vs time with the D command. There may be some other way to do it more directly but I am not aware of it. You can apply acceleration fields (e.g., gravity) with the ACEL command.

 

[12civil34]

Hi terio,

Thanks for your response. For the gravity force do I need a seperate analysis first and then do the next transient analysis having the results from the gravitational one? I'd appreciate you response.

 

[Drej]

Terio is correct. You cannot apply an acceleration time history directly using ANSYS. You will need to apply the base motions as displacements using an appropriate method - be very, very careful with deriving displacements from base accelerations...

An appropriate method for applying the displacement base motions would be to use the D command and apply the motions using a Table reference (see the D command). For the gravity response, do an initial dynamic step (ANTYPE,TRANS) with ACEL (split into at least 5 substeps to avoid residual dynamic effects) with time integration switched off (TIMINT,OFF). Then carry out your dynamic step with time integration initialised.


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

 

[12civil34]

Hi Drej,

Thanks for your valuable response. I have another question regarding the gravity. As I said I have assigned density of material to my concrete material, now the point is does ANSYS apply the gravity to this value or I need to introduce a seperate mass using the mass element?

My second question is that I want to run two subsequent ground motion analyses and I want to keep and save the result of first one such as the deformations, stresses, nonlinearities (in a word everything) and then continue analysing with the second one. How should I proceed with such analysis?

I truly appreciate your guidance.

 

[Drej]

As long as you define density for your elements, this will be sufficient for gravity to act.

For your second question, it's possible, but I wouldn't advise doing this since the results file would be very messy. Consider doing a separate analysis.

Cheers.


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

 

[12civil34]

Hi Drej,
Thanks for your response. The point is that my structure goes nonlinear under the first ground motion and I wanna see with this nonlinearity how it will respond under the second earthquake. Thats why I have to carry on the state of the structure at the end of first ground motion as the initial state of the structure for the second analysis under second ground motion.

Would you please guide me how I can do this analysis as stated. I truly appreciate your response.

Best

 

[Drej]

Hmmm. This appears to be a rather strange analysis, in that ordinarily you would never consider this. Ordinarily.

Are the ground motions separate i.e. are they taken from separate/independent seismic events? If so, you cannot simply analyse these "one straight after the other" since physically the ground motion (specifically velocity) at the end of one and the beginning of the other will be specific to the seismic event, and hence the analysis itself will be nonsense. If you tried to do this you would see a step change in velocity at the end of the first event which would be completely artificial, and hence nonsense. The evidence of this would be massively artificial base accelerations.


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

 

[Drej]

I should also ask how you know that your "structure goes nonlinear" following the first ground motion?


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

 

[12civil34]

Hi Drej,

The layout of the problem is as following:
I have a safe structure which under goes a seismic event (acceleration input) and it might get nonlinear, I have defined nonlinear behavior for my concrete and reinforcing steel and I can check whether the concrete has cracked (gone nonlinear due to cracking) after the first ground motion.
Later I apply this second ground motion. If I want to give a real life example it would be the first ground motion is the major earthquake and the second one would be the aftershock of that major arthquake. What I want to see is whether my structure which has sustained nonlinearities due to the first ground motion, can sustain the loads induced by the second ground motion ( before i go and fix it)or it may have some failures. So as you can see I have to keep the whatever results I have in my elements and run the second ground motion on that one. But obviously there is a grace period between the two analyses where no acceleration is applied , since there is always some time lag between a major earthquake and its after shocks.

 

[12civil34]

Drej,

I also have another question to clarify the way we should input the ground motions. You mentioned that its impossible to apply accelerations in ANSYS and I should apply displacements using the D command. but I am looking at the D command and I can see that there are ACCLX,ACCLY,and ACCLZ as items in D command which are accelerations in three directions, can't I use them to apply my acceleration input?

I remember that I saw another thread from you saying that the earlier versions of ANSYS didn't support acceleration input but after V.8 acceleration can be defined. As I ahd mentioned earlier my ANSYS version is 12.0.1. The reason I have this concern is that I am double integrating acceleration data I have ( as you guided me to) and when I run it, the results seem really wierd.

I' truly appreciate your input for these last three questions.

Best regards

 

[Drej]

I've not used ANSYS 12 but if you're now able to apply accelerations directly then this is a welcome addition to the code.

Raw acceleration data, especially from test accelerometers, is notably "noisy" and can contain frequency content which is either artificial or unwanted in the analysis. Check the data and consider using a suitable filter for the time histories. Not sure what you mean by "weird" but I suspect those results may be caused by your double integral and the fact that the displacements aren't baseline corrected. They need to be to be meaningful for displacements.

The analysis of the aftershock is going to be tricky. If you run the first analysis for say 10 secs, then you will need to apply a period of time to stabilise the model before applying the second, since the model will still be responding dynamically after the first event (non-zero velocities). You will need to consider an intermediate step here to bring the whole model back to zero velocities. Consider using a step where you apply zero loads other than maintaining the gravity load (the GRAV load should still be maintained during the first event). This period of "non-load" will need to be enough to achieve this in the model and I suspect you may need to run a series of tests (of different time lengths - with time integration still active) to ensure this occurs. Then check the model. Once the model stabilises, run the second event, but be very careful of step changes in the response (other than that caused by the second event) when doing so.

Hope this helps. Good luck.


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