Nonlinear transient dynamic seismic analysis in ANSYS 1

[brc01]

Thank you Dreaj for your valuable replys .The following thred discussed combining seismic responces using SRSS etc.

http://eng-tips.com/viewthread.cfm?qid=18095

My present problem is:

I need to do nonlinear full transient dynamic (so all modal methods and response spectrm method are exluded from consideration)seismic analysis of a piping system.

I have Acceleration-time history of ground motion.

The ACEL command in ansys for applying acceleration applys the acceleration to the entire structure in global X/Y/or Z directions.

But what I want is to appply acceleration only at the points where the piping is connected to the ground.

Apart from using BIG-MASS method,is there any method to apply Acc-time history in nonlinear transient dynamic analysis?

 

[Drej]

> Apart from using BIG-MASS method,is there any method to apply Acc-time history in nonlinear transient dynamic analysis?

No. What you can do is take your acceleration time history and integrate back twice (ANSYS can do this for you, see the INT1 and INT2 functions - alternatively set up a spreadsheet to do this) to get a displacement time history. Then apply these in your transient analysis through a table (*DIM & D commands).

Cheers,

-- drej --

 

[brc01]

Hi dear Drej,
Thank you for your prompt reply.

A doubt..
DO you think that applying acc.time history with ACEL commandin ANSYs (for ex using a do loop) to unconstarined structure in (nonlinear) transient dynamic analysis is correct method to simulate ground motion due to earthquake?I feel it is wrong coz it shakes the entire strcture in global dir.ns instead of shaking just at fixed base.

Another Q.

If I want to do nonlinear transient dynamic analysis of piping with internal pressure(earthquake accc vs time histroy ) in ABAQUS/standard using kineamatic/combined hardening ,using Direct dynamic analysis,what steps should I follow?

Can I apply fixed BCs at the point where the pipe is fixed to the ground in modal definition,and then in static STEP-1 apply interanl pressure,in Dynamic step-2,apply Acc-time history as amplitude curve,to the same fixed end (where fixed BCs were applied in modal def)??

Or can I simply apply acc time history to one end(where it is supposed to be fixed to the ground) of free-free pipe and also simultaneously apply internal pressure.

I want to see ratcheting of pressurized pipe due to cyclic earthquake loading.

Any clues??

Buest regards
--BRC--

 

[Drej]

> DO you think that applying acc.time history with ACEL commandin ANSYs (for ex using a do loop) to unconstarined structure in (nonlinear) transient dynamic analysis is correct method to simulate ground motion due to earthquake?I feel it is wrong coz it shakes the entire strcture in global dir.ns instead of shaking just at fixed base.

I think using ACEL would give an incorrect response, especially so if it was unconstrained. This has been argued before, and I believe the general feeling then was the same - the two methods (using ACEL and the large mass method) are not equivalent. Some people argue that they are - I'm not one of them.

> If I want to do nonlinear transient dynamic analysis of piping with internal pressure(earthquake accc vs time histroy ) in ABAQUS/standard using kineamatic/combined hardening ,using Direct dynamic analysis,what steps should I follow?

You should post this query in the ABAQUS forum.

>Can I apply fixed BCs at the point where the pipe is fixed to the ground in modal definition,and then in static STEP-1 apply interanl pressure,in Dynamic step-2,apply Acc-time history as amplitude curve,to the same fixed end (where fixed BCs were applied in modal def)?? Or can I simply apply acc time history to one end(where it is supposed to be fixed to the ground) of free-free pipe and also simultaneously apply internal pressure.

Do the latter. Remember that your time history is a boundary condition and is direction dependent. You apply the time history to the ends of the pipe for each direction that you have data for, so you don't need to fix these directions. The other directions - if applicable - must be constrained. I would apply the internal pressure in load step one, and then apply your time history in subsequent load steps.

> I want to see ratcheting of pressurized pipe due to cyclic earthquake loading.

This is another query completely. One step at a time. Understand your dynamic analysis first with a simple material model, then build to something more complex.

 

[cloche]

Hi all, I'm also really interested on the trans non-lin analysis of an earthquake. I deal with a structure enclosing conductor's bars in an electric station, it's something like a piping system also. The problem I have is to translate the Italian Seismic Norms into something usable: they give the SPECTRUM of displacement vs freq, so I have to get back to the time-dependent D=f(TIME). I thought to use an Inverse Discrete Fourier Transform, but do you know which convention does ANSYS expects for normalizing the phasors? The Fourier Transform has more than one possible equivalent definitions, but anti-transforming with a different def would give uncorrect results... Do you know what is the definition used by ANSYS ? Thanx in advance - Claudio

 

[cloche]

I forgot...
to brc01: Drej is right, you should NOT apply ACCEL uniformly on the structure in order to get its correct response: you would disregard internal mutual effects because the effect would be as if you specify the same a=f(t) on all the points of the structure; a=f'(t) in the unexcited points depends instead on the structure itself. think of infinite stiffness and zero damping -> then wherever you eccitate the structure, the whole will respond with the same accel and displ amplitudes; but if you think of near-zero stiffness and infinite damping -> then if you excitate at the base, nothing must happen (I simplify...), whether if you apply uniform ACCEL, every point would accelerate and displace in the same way, which semms to me to be a nonsense...

 

[brc01]

Drej,
Thank you for your kind reply.
(BTW,I posted the ABAQUS part of question in ABAQUS forum too but nobody replies.so I would like to discuss it further here with you and all)

>>You apply the time history to the ends of the pipe for each direction that you have data for, so you don't need to fix these directions. The other directions - if applicable - must be constrained.



The structure is actually completely fixed to ground at one end say end " A"

Am I right in saying that in dynamic analysis (unlike in static analysis)here is no compulsion to prevent rigid body motion in all dof?

If I have to apply excitation only in say Y direction at the fixed end , I would apply the acc-time history in that direction at that point and leave all other dof free everywhere.

Will the responce from such a scenario be different from a case where Y acc is applied(keeping Y dof free) and other dof are fixed ?

>>The other directions - if applicable - must be constrained. I would apply the internal pressure in load step one, and then apply your time history in subsequent load steps.

So I understand that in load step 1 for applying internal pressure :fix all dof at "fixed" end and apply internal pressure.

Load step 2: Modify BCs applied in the step1. Remove fixity only in the direction(s) you need to apply ACC keeping fixity in other dofs.

Right?

> I want to see ratcheting of pressurized pipe due to cyclic earthquake loading.

>>This is another query completely. One step at a time. Understand your dynamic analysis first with a simple material model, then build to something more complex.

I agree with you.one step at a time.
But the query is not completely out of context .
When I have internal pressure and cyclic excitation due to earthquake in my actual problem I mentioned ,when the load is high enough to induce plasticity(the very reason for choosing direct time integration for my model rather than a modal based method)ratcheting takes place due to accumulation of hoop strain in the pipe.

Your suggestions would be highly appreciated on this subject.

Best Regards,
---BRC---

 

[cloche]

If you leave DOFs unconstrained, you should ensure that no component of load (neither external nor internal) develops along those DOFs. Otherwise, you will get "DOF XXX is higher than allowed" or a message like that (I don't remember the exact phrase) during the calculation; during the solution pre-computing, you would receive a warning "small equation pivot term" or even "zero equation pivot term". The solution can still be achieved with small pivots, but not when the zero-pivot condition remains during the iterations (i.e., is not due to numerical momentaneous condition but is due to structure setup). You can set "soft springs" if you want absolutely to leave your structure "free"

 

[Drej]

> The structure is actually completely fixed to ground at one end say end " A". Am I right in saying that in dynamic analysis (unlike in static analysis)here is no compulsion to prevent rigid body motion in all dof?

No. You still need to prevent rigid body motion.

> If I have to apply excitation only in say Y direction at the fixed end , I would apply the acc-time history in that direction at that point and leave all other dof free everywhere.

No. You need to apply the boundary conditions in your model that are in your physical system. If all DOF in your piping system are fixed then you must fix all of them in your model. *******HOWEVER******, you have a time-history to apply. You must apply this time history to the end of the pipe in the relevant direction it was measured in. If you have time history data for the X, Y and Z directions, you must leave these DOF free at the nodes in which you apply the time history. The *****OTHER***** DOF must be fixed according to how your structure is actually fixed and to avoid rigid body motion..

 

[brc01]

Thank you Drej and Cloche for giving valuable insights.

I have a simple question in using Big_Mass method,which I never used before.,but am going to use now.

How should this big mass (M)(~ 10^6 times structural mass)be attached to the structure (pipe)at fixed end to apply force(F=Ma)input to it? As a point mass element at a single node?
Or shall I have to model a really big 3D block(if I do this again I get into trouble connecting 3D to shell model of pipe !)

Regards,
--BRC--

 

[cloche]

I think the first way is correct: you put a MASS elem on the desired node, then give its real const a very high value of mass.
BE CAREFUL if you have defined Rayleigh damping factors: alpha is proportional to mass, so if you use "big mass" method you will get fictitiously and misleadingly high damping !!

 

[brc01]

Cloche,
You are right again!
Thanks!

--BRC--