How to apply Earthquake excitation in Abaqus CAE

[IRSHADQUR]

Hello everybody

I want to know that how can i apply earthquake excitation (acceleration) in Abaqus CAE.
Plz kindly tell me or refer me any links that can explain the procedure to apply this excitation as i am just a beginner in Abaqus.

With Regards
Irshad

 

[kalamatajpm]

Dear Irshad,
I am not a new user of Abaqus, but I have the same problem to you. It is really complicated to input an earthquake motion. I tried to do it but ....it's Aborted.
take some ideas from the following presentation

http://www.google.gr/url?sa=t&rct=j&q=&esrc=s&source=web&cd=14&ved=0CEQQFjADOAo&url=http://

http://www.ae.gatech.edu/people/jcr...Ao8r_5iz5C5k9cw&bvm=bv.45645796,d.Yms&cad=rja

 

[IRSHADQUR]

Well its working fine for me now.........kindly illustrate your problem may be i can help u in this regard (although am a new user)

 

[kalamatajpm]

It is now ok for me too. Thank you a lot.
Finally, I defined at Load-->Tools-->Amplitude-->Tubular--> my ground motion.
After this I defined as a boundary condition the acceleration of interest and I put there a number which is sth like a scaling factor.
I also removed in this step the boundary conditions in the acceleration direction.
That's all.
be careful at the step properties to put a fixed increment equal to the time step of the ground motion and as time period the total time of the earthquake.
I write these in case someone else is searching about it in the future.
Best regards

 

[Drej]

be careful at the step properties to put a fixed increment equal to the time step of the ground motion and as time period the total time of the earthquake.

I would be very cautious about applying a general rule 'to put a fixed time increment equal to the time step of the ground motion'. The time step magnitude needs to ensure that the response you are interested in is captured. If the the time step is too large the analysis will not pick up this response. If this is too small it may produce excessive run times and/or cause numerical issues. Fixing the time increment also requires experience to ensure the model is responding correctly. The ABAQUS manual gives guidance on time step usage, I would definitely recommend you take a look, especially if you have any non-linearities in your model.


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

 

[IRSHADQUR]

I was about to write the same thing that fixing time period can cause problems in analysis and one has to be cautious.
How about automatic time increment:
My time history has a time step of 0.0041 for each new acc. value. I used automatic time increment and the software is using 2*10^(-5) sec as stable time increment. However i am getting the output at every 0.0041 sec because this time is also the time step of the instrumentation i have used for the experiment.
Dear Drej what do u think abt this? is it ok to use automatic time increment?

 

[Drej]

IRSHADQUR, there is a lot to consider, depending on your model. The time step size and the resolution of modes in the model is loosely related to the nyquist frequency of the data, in that you can only resolve models of half the nyquist (which is related to the sampling rate of the data). Your timestep (dt) seems very small, but you don't state if this is the initial or the min dt you're using in line with automatic incremeentation.

Firstly, do a modal analysis and establish the main mode/s of interest for you in your model. Knowing this information, you will need to then try and resolve the frequencies you are interested in by setting the time step.

As a rule of thumb (and no more), use the following:

If your model is linear and you wish to resolve the frequency (f) of the highest mode of interest in the model, use max dt = 1/(5f)
If your model is non-linear (ie contact, plasticity, large strain), consider max dt = 1/(20f)

Obviously the higher frequencies are more difficult to resolve in that these require a smaller time step.

The 1 and 5 in the equations above attempt to resolve a sinusoidal wave by suggesting that for linear models this can be resolved by using 5 points for the (sine) wave cycle. Similarly, 20 points for models involving contact and large non-linearities. It's fine to use automatic incrementation as long as you put the correct controls in place for this ie you limit the dt to ensure you capture your main response frequency as I've described.

Unfortunately, you also need quite a lot of experience to make sure your model is behaving correctly, which takes time. The above is only a short summary of what needs to be considered, but hope this helps.


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

 

[IRSHADQUR]

Dear Drej
My problem is a contact problem in which i want to get the results for horizontal and vertical response of the structure. (Especially acceleration values).
I cant see anything in step properties to show the min dt. However we can specify the max dt. The max frequency i am interested is 1/0.007 = 142 cycles/sec.
My problem is a contact problem. (Why i cant do frequency analysis for a contact problem. I am using some other software for frequency analysis. Abaqus says that interactions cant be used in frequency analysis)
So based on thumb rule max time increment should be 1/(20*142) = 0.00035 sec.
Now during whole of the analysis procedure the stable time increment was constant and was equal to 1.96e-5.
(1) Do i need to make it constant and equal to 0.00035? (may be abaqus will have some convergence problem as i have seen earlier)
(2) or if i get the output after every 0.00035 sec then it will be ok.
I really appreciate your help in this regard.
Regards

 

[Drej]

I'm thinking, Are you using Abaqus/Explicit? It sounds like you are when you suggest the "stable time increment" (and may explain some of your post above, including why it's so small). In this case the time increment calculated by the code has to be maintained for stability, and is calculated based on a critical element dimension in your model and the element density. The dt can be artificially increased as long as you're careful about inertial effects (but that's another issue). I would suggest that if you're using Explicit then try and maintain the dt set by the code (unless run times are giving you problems) since in explicit the code will largely control the incrementation for you using auto stepping. So, in answer to your questions above: (1) No (2) Yes.

Incidentally, you can only carry out a frequency (eigenvalue) analysis on a linear structure, which is the reason why Abaqus is giving you those messages regarding contact interactions (I'm guessing you have standard contact or something else which makes the contact non linear). You can linearise your contacts (bond) to get round this if it is applicable.


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

 

[IRSHADQUR]

Thx alot for replying.
Yes i am using abaqus explicit (Sorry i did not mention it before)
Actually my structure is a rocking wall structure and there will be gap opening and closing phenomenon at the intersection of rocking wall and foundation which means that the response will be non-linear. Anyways thx alot again for guiding me

 

[Sorourian]

Dear IRSHADQUR,

I want to analysis a steel frame with abaqus explicit, at the first step I decided to model a simple column in abaqus explicit, would you please refer me a link that explain how to use abaus explicit?
Regards
Samin

 

[IRSHADQUR]

Dear Samin

I am also beginner in Abaqus . As for as i know, for the explicit analysis u need to select the Step (after initial step) named as Dynamic, Explicit.
However the choice of explicit or implicit depends on ur problem type. If its not a complex (Contact) or highly dynamic problem then u can use the Dynamic, Implicit method. Anyways it all depends on the step type. Static, General for quasi-static analysis and Dynamic, explicit for dynamic analysis. I dont really know abt a link where u can find step-by-step procedure. Best of luck and do ask if u need to know some other thing. Cheerz