Transient analysis with birth and death elements

[hercend08]

Hi,

I have been working on disproportionate collapse of buildings (a simple 2D frame), and trying to simulate the dynamic effects of a sudden column removal in ANSYS 11. I have been working on it without success for the past two weeks and I genuinely do need help.
I have created 3 different loadcases.

For the first, I have applied all vertical loads. then write the loadstep
for the second, I am trying to get KILL a column using birth and death option by selecting the column from the graphical interface (In this loadstep, I'm not supposed to have the column). However, it does not allow me to write the loadstep as I have done for the previous one.
An error message appearing, suggesting me to solve the loadstep without Writing LS (just as i have done for the first one). therefore, I havent been able to create the third loadstep.

So my problem is to know whether it is possible to use Birth and Death Elements with different LS. If there is any other technique to simulate the sudden column removal.

Thanks so much
hercend

 

[rickfischer51]

First, are you running a transient analysis, or simulating a transient condition with multiple static load steps? Are you killing a particular column, or are you looking at column stresses and selecting the one with the highest stress?

I would not do this interactively. I would write a script and run it with the /INPUT command. Lets say you had 10 columns. Make a component from each column called COLUMN1, COLUMN2,,, etc. The script might look something like this:

/prep7
! build model
/solution
antype,static,new

!apply loads and BC's

time,1

solve

*do,loops,1,10

/post1
set,last
ncount=ndinqr(0,14)
*dim,ndata,,ncount,5
*dim,cdata,,10

*do,cnum,1,10
cmsel,s,column%cnum%
nsle,s
*vget,ndata(1,1),node,1,nsel
*vget,ndata(1,2),node,1,s,eqv
*vmask,ndata(1,1)
*vscfun,smax,max,ndata(1,2)
cdata(cnum)=smax
*enddo

*vscfun,cmax,lmax,column(1)

allsel

/solution
antype,,rest
time,1+loops

cmsel,s,column%cmax%
ekill,all

allsel
solve

*enddo

This will kill the column with the highest stress in each of ten load steps. You could also kill only columns with stress over a given value, or kill the columns in a specified order, or what ever you want. This is not tested, so it may need some debug, but the concept is there.








Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[hercend08]

Thanks so much,
I am simulating a transient condition with multiple static loadsteps and willing to kill a particular column in the second loadstep.
The Time at the end of first loadstep is 5
and time at the end of second loadstep is 5.001 (its here that I am willing to kill a particular column; nothing to do with its stress or force conditions)
time at the end of the third load step is 7. I am willing to have the same time increment of 0.001 (for argument sake).

Also, I am not really familiar with ANSYS script. That is the reason why I have been running away from it.

Thanks so much

 

[rickfischer51]

If you are running a static analysis, the time numbers have no physical meaning, unless you are running a creep material. They are just numbers, with no unit significance. You can set them to anything you want.

Scripting is way cool. It gives you a list of what you actually did. It's a record to document your work. And it offers repeatability. Learning the APDL commands opens the door to analysis scenarios limited only by your imagination. You will have unlimited access to the database, with the ability to post process on any result, create your own results, etc. You can apply very complex loads, simulate unusual material behavior, apply a failure criteria, etc. Your boss will be impressed, your coworkers will envy you, and women will swoon. OK, I made up the last part, but you get the idea.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[hercend08]

Thanks so much for your reply and advices. I will consider them.
Nevertheless, I would like to know whether it is possible to run both static and transient analysis in one solution.
Say LS1 : static analysis (time at the end of loadstep: 3)
LS2: transient analysis (time at the end of loadstep: 4)
solve> from LS file 1 to 2
I am having some error using this process, so I would like to know whether there is any other technique to overcome this.

Thanks

Hercend

 

[rickfischer51]

I dont know, I've never tried, but I doubt it.

If you want a load step without dynamic effects, give it a very short time, i.e. time at end of load step is .0001. As I said above, the time for a static analysis without viscoelastic or creep effects has no physical meaning. If you are trying to establish initial conditions, try the IC command.

Rick Fischer
Principal Engineer
Argonne National Laboratory