Thanks for interest Stringmaker.Yes I mean acceleration vs time, in Italy we call it "accelerogramma".I am beginner of Ansys and I don't know how to apply a table of 2000 points acceleration vs time at the base of my structure in a transient analysis,I need a time-history response. A help would be very pleasant!
You've got a little bit of work ahead of you then. Somehow you are going to have to store all of the time-acceleration information in an array within Ansys. Before we go any further do you have a function describing your data? Or a spreadsheet containing 2000 data points? What form is it in now and I'll try and tell you how to get that into Ansys.
Thanks still, Stringmaker.I have exactly 1536 points accel.-time on a notepad file (txt), they are a record of earthquake, therefore there is no function describing them. Someone says it's not possible giving accelleration vs time in Ansys, but only displacement vs time in a transient analysis, i would to know!
Hi,
it depends: in v.11.0 Ansys has added the ability to handle accel BC in a transient analysis.
If you're using v.10 or lower, then yes, unfortunately you will have to shift from accel to displacement, and this won't be very easy...
Thanks cbrn.Unfortunately I'm using Ansys CivilFEM 9.0, so I can only use displacement vs time, but my problem is the same: insert a displacement vs time point table in a transient analysis and obtain time history. Help please!!!
Micmaf,
Can you not integrate your data twice with respect to time and get the displacement for each point? I don't have any references handy here at home but I seem to remember this being fairly simple. You should be able to do this in Excel or even using the *VXXX series of commands within Ansys. Once you have this, you can simply apply the displacement using tabular data of displacement vs. time within Ansys.
Hi,
ah, sorry, I misread the post, I was thinking about the normated spectra for earthquake as in the italian D.M. 14/09/05...
Yes, as Stringmaker says, if you have a time-dependent acceleration history, then you can perform a double integration. You will have only one "problem" in assigning appropriate values for the integration constants, but you can think about them as being initial velocity and displacement, so I believe you can fix it to zero.
But the time history is discrete, it's not written as a function, so you will have to make some assumption in re-building a piecewise function connecting groups of time points: the simplest is to connect only two successive time points in a linear fashion, so if you have n time points you will build n-1 functions of the type ai=mt+q, then you will pass to velocities vi=(1/2)mt^2+qt+c1 (where you can set c1=0 if you consider that the earthquake begins from a "stillstand" state), and lastly to displacements si=(1/6)mt^3+(1/2)qt^2+c1t+c2 (where you can drop the two last terms). The displacements have to be considered as "incremental": at time point t, the displacement s[t] is the sum of s[t-1] and si, and so on. It's tedious to do by hand, but almost immediate with Excel.
Hope this helps and that I didn't miss something...
Yes, I can integrate my data twice with respect to time obtaining displacement vs. time, but someone can explain me how create a table with, we say, 2 columns and 2000 rows, where the first column contains values of the time and second contains values of displacement and then how apply this table in a transient analysis avoiding,in this way, to do 2000 steps? Thanks for your help Stringmaker ans cbrn.
Then, in Ansys, go to Parameters -> Array Parameters -> Read From File -> Table
and input your text file, while assigning it to a table-variable.
When it comes to assign D boundary conditions, instead of an explicit value select "existing table" and give the previously defined table name.
You need only one step but many substeps (depending on which is the max response frequency you expect to be significant for your system - in this sense, a previous modal analysis is very helpful).
You should be able to export something from excel rather easily. Make sure your file is space (not tab) delimited. Ansys normally doesn't like reading file delimited by anything other than spaces.
Cbnr,your help has been me very useful! A last thing, when I create the table in which I will insert the text file, must I give Var1 = Time, Var2 = UX (in my case I had to assign displacements in x direction varying in the time), that is, for Var2 I had to give name of my variable according to the codings Ansys.It's right????????
Hi,
1- if you use the APDL commands, the syntax given by Stringmaker applies: you can see that the "*DIMensioning" of the table calls "TIME" the first variable and "X" the second one.
2- if you use the graphical interface, as you say Var1 (row) is TIME and Var2 (column) is X (not UX, if I'm not wrong).
