Base Excitation Modeling using Ansys

Ansys is quite well suited for base-excitation problems in structural engineering.  Implicit dynamic capabilities are included in all Ansys licenses.  A user who is reasonably familiar with static analysis in Ansys and has adequate understanding of structural dynamics to have at least a general understanding of the problem to be solved and what might be a reasonable solution should be able to do a dynamic analysis without major difficulties.

Pre-processing:

There are no differences between modeling an implicit dynamics problem and modeling a static problem in Ansys.  The model can be built using any of the structural elements, including solids, shells, links, beams, pipes, etc.  A model created for static analysis may be used for dynamic analysis, although dynamic modeling may use slightly different assumptions and will require the inclusion of certain other details of the structure, such as masses.

There are some special elements that may be useful in a base-excitation model.  The effects of non-structural items, such as RTUÕs or equipment, may be accounted for using the structural mass element (MASS 21).  Be careful to distinguish between the thermal mass element (MASS 71) that as opposed to the structural mass element.  The combination elements include springs, dampers, and pre-tensioning that may be useful in certain problems.

One of the most important considerations in dynamic analysis is using consistent units for length, mass, gravity and other accelerations, and material properties.  Any system of units may be used, as long as it is consistent and used throughout the model.  This can be especially tricky when using English units.  The following table may be helpful (from DRD Technology, http://www.drd.com/searchable/techsupport/units.html).  It is also important to remember that unlike a static analysis, time serves as more than a counter and has meaning.

Loading and Solution:

The procedural differences between static analyses and base excitation analyses are in the assignment of solution options and loads.  The University of Alberta Department of Mechanical Engineering has a good description of this process on the web: http://www.mece.ualberta.ca/tutorials/ansys/IT/Transient/Transient.html.

This process is not difficult, although it may be time consuming to apply a complicated base excitation with many steps (i.e. any real-world excitation).  The simplest way to modify a load step is often to edit the .sox file using any text editor instead of using the GUI and re-writing the file.  The figure below points out some of the important parts of this file.  The red text is commentary pointing out some of the important parts of this file.  The tutorial includes mention of a good rule of thumb for the time resolution required for a particular problem:  1/20^th the period of the highest mode of interest.

The procedure for using the full solution method instead of the reduced method (as described in the tutorial) is very similar to the procedure outlined in this tutorial, except that master degrees of freedom are not defined, and there is no need to expand the solution to see full results.

When applying acceleration due to gravity, remember to apply it in the direction of the reaction to gravity (i.e. upward), not the other way.

Base excitations are best applied in terms of displacement at a given time rather than in terms of accelerations.  When an acceleration load is applied in Ansys, it is applied to the entire structure, as opposed to only the base.

Viewing the results:

There are two ways to animate results in Ansys.  Each can be useful for quickly inspecting a results set.  The Results Viewer (in the General Postprocessor menu) allows animation of the deformed shape of the structure over time with contours showing a selected nodal result item as applicable to the elements used in the model (displacement, stress, strain, energy, or contact status) and gives the user the ability to stop at a particular sub-step or to jump to a particular load step.  The Animate Over Time option under Plot Controls -> Animate creates the desired number of frames over the desired time period showing deformed shape or a nodal result item (displacement, stress, strain, energy, contact, etc.).  Animations with a very large number of frames may bog your computer down, so be aware of what you are asking it to do!  The animation here was created using Animate over time, and results in a very large AVI file (9.5 Mb).  The Animate option is not appropriate for dynamic problems (or nonlinear static problems, for that matter).

The General and Time-history postprocessors work the same way as for static analyses.  The time-history postprocessor (including its ability to export data in text form so that plots of a quantity over time can be manipulated using other software more suited to this purpose) can be very useful.

/COM,ANSYS RELEASE  6.0    UP20010919       17:54:27    07/24/2003 /NOPR /TITLE,                                                                         _LSNUM=   2 Load Step Number 2 ANTYPE, 4   Analysis Type 4 = Transient TRNOPT,FULL,,DAMP BFUNIF,TEMP,_TINY   DELTIM, 1.00000000E-02,  0.00000000    ,  0.00000000    , Initial, Max, and Min time step sizes KBC,     0 KUSE,     0 TIME, 0.200000000 Time at end of step TREF,  0.00000000 ALPHAD,  0.00000000 BETAD,  0.00000000 DMPRAT,  0.00000000 TIMINT,ON  ,STRU   CRPLIM, 0.100000000    ,   0 CRPLIM,  0.00000000    ,   1 NCNV,     1,  0.00000000    ,     0,  0.00000000    ,  0.00000000   NEQIT,     0   ERESX,DEFA OUTRES, ALL, ALL, Write the complete results set for every substep ACEL,  0.00000000    ,  0.00000000    , 386.4   Acceleration vector OMEGA,  0.00000000    ,  0.00000000    ,  0.00000000    ,     0 DOMEGA,  0.00000000    ,  0.00000000    ,  0.00000000 CGLOC,  0.00000000    ,  0.00000000    ,  0.00000000 CGOMEGA,  0.00000000    ,  0.00000000    ,  0.00000000 DCGOMG,  0.00000000    ,  0.00000000    ,  0.00000000 IRLF,  0   D,      1,UX  , 0.500000000    ,  0.00000000 D,      1,UY  ,  0.00000000    ,  0.00000000    D,      1,UZ  ,  0.00000000    ,  0.00000000    D,      2,UX  , 0.500000000    ,  0.00000000    D,      2,UY  ,  0.00000000    ,  0.00000000    D,      2,UZ  ,  0.00000000    ,  0.00000000    D,      3,UX  , 0.500000000    ,  0.00000000    D,      3,UY  ,  0.00000000    ,  0.00000000    D,      3,UZ  ,  0.00000000    ,  0.00000000    D,      4,UX  , 0.500000000    ,  0.00000000    D,      4,UY  ,  0.00000000    ,  0.00000000    D,      4,UZ  ,  0.00000000    ,  0.00000000                     Magnitude of BC           Direction and type of BC  U=disp., F=force, M=moment         Node number BC type Ð D=displacement, F=force/moment /GOPR