Imposing acceleration time histories 1

[andreamordini]

As long as I know, it is not possible to an acceleration time histories to a nodes in a transient analysis in ANSYS. Tipycal example a multi support analysis af a bridge where each pier has a different excitation.
The same procedure is possible in ABAQUS.
My questions:
1- How the procedure is performed from the numerical point of view?
2- Is it possible that the acceleration time history is in ABAQUS simply double integrated and applied as a displacement time history?
3- Both the software are high level software. Why this different between ANSYS and ABAQUS?

Thanks,
andrea


-------------------------------------------
Dr. Andrea Mordini
Civil Engineer
Ph.D. in Structural Mechanics

http://www.andreamordini.com

-------------------------------------------

 

[cbrn]

Hi,
Ansys IS able to apply accel time-variant loads in a TRANS analysis:
"5.3.5. Apply the Loads
[...] The loads shown in Table 2.5: "Loads Applicable in a Static Analysis" are also applicable to a transient dynamic analysis. In addition to these, you can apply acceleration loads in a transient analysis (see DOF Constraints in the Basic Analysis Guide for more information)."

However, displacement time-histories are of course the twice-integration of accel time-histories, given the appropriate boundary conditions (initial speed, initial displacement).

Regards

 

[meshparts]

Hello,

I was hopping cbrn was right, but at the link cbrn provided I couldn't find any possibility to define an acceleration at nodes. So, cbrn, can you provide more information about how to define a direct acceleration at nodes? This would be grate, if possible.

Of course integrating the acceleration 2 times would give the same results, but a direct way to apply acceleration would be very comfortable in Ansys.

Regards
Alex

 

[cbrn]

Hi,
I don't know if there is a GUI path for that; however:

D,<node>,ACCX
D,<node>,ACCY
D,<node>,ACCZ

Warning: ONLY in transient analyses, as mentioned.

See the help file about "D" command.

Regards

 

[meshparts]

Thanks cbrn! A star for you! Actually it's elementary, but once again, I will always learn about Ansys!

Regards,
Alex

 

[cbrn]

Hi,
I agree Ansys' people could have invented something more (much more !!!!) practical, more (much more !!!!) intuitive and less (much less !!!!) hidden...
However, the important thing is that they let us have the job done, so... ;-)

Regards

 

[andreamordini]

Many thanks cbrn! I use the version 10 and this feature is undocumented. Nevertheless, it works.
I tried to perform a comparison with OpenSees and I got the same results. Since in OpenSees is documented that double integrastion is performed, I would conclude that this method is used in ANSYS as well.

Personal comment: you are right, cbrn, when you say "the important thing is that they let us have the job done, so..." but if I have to ask a forum (waiting some days for the answer) to have the documentation, I can not be satisfied of ANSYS. My response about this software is everyday worse.

andrea

-------------------------------------------
Dr. Andrea Mordini
Civil Engineer
Ph.D. in Structural Mechanics

http://www.andreamordini.com

-------------------------------------------

 

[cbrn]

Hi Andrea,
I disagree: most of the times, it's "only" a matter of carefully reading the help system (in v.11). Though it is extremely complex, it is also extremely complete.
To return to the original problem: yes, it's hidden in v.10 because most probably it was a "beta" feature. In fact, it is listed in the "v.11 improvements". Up to v.10 I personally performed the double-integration. So, it's great you performed the "double-check" with another system, so you're sure of your results in this case. But consider them with care in other analyses, unless you upgrade to v.11 (which I recommend, by the way).
Regards