Harmonic Analysis Loading

[Stringmaker]

I have what is probably a simple question but one which for the life of me I cannot quite come up with on my own. I'm performing a harmonic analysis using Ansys 10 on an electronics chassis with some electrical components. My model consists of beams, solids, shells, and masses. There are four points at each of the chassis corners where it is fastened into an avionics rack. Ultimately, my goal here is to find the displacements in various places when it is excited with a 0.1g sine input from 0 Hz to 2000 Hz.

My question is how does one go about applying loads to these four attachment points? These could be considered the base of the model so to speak. I have tried applying only an inertial load of 0.1g at these points in the direction of interest and the model seems to diverge. In a harmonic analysis can one apply both loads (acceleration in my case) and constraints at the same point and both will be considered? Or is there a different methodology that needs to be taken here? It seems like until I add constraints convergence is something that is not in the cards for me.

Thanks for reading!
-Brian

 

[Drej]

Brian - first of all, you can't apply your 0.1g load directly. You'll need to convert this into real (and imaginary if necessary) components for your harmonic analysis, specifically displacement. Where you apply this depends on where it has been measured on your system. Remember that all loads applied are assumed to vary sinusoidally (even gravity, temperature, etc.), so you only need to apply the maximum value. You will still need to apply boundary conditions for the other directions to stop rigid body motion of the model. If you have g loads available for the other directions, apply these instead, but again make sure you have your model properly constrained. Some general points to remember:

Input can be:

=> Harmonic loads (forces, pressures, and imposed displacements) of known magnitude and frequency.
=> May be multiple loads all at the same frequency.
=> Forces and displacements can be in-phase or out-of phase.
=> Surface and body loads can only be specified with a phase angle of zero.

Hope this helps.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Stringmaker]

Drej,
Thanks for the reply! I do have one question...how does one go about converting and acceleration to a displacement? Since I'm covering a frequency range here I don't believe that the displacement will be the same for each frequency even though the acceleration (0.1 g's) will be.
Would applying the harmonic force which would provide me with 0.1 g's acceleration be a better way of applying the load that I'm looking for?

Thanks for your help,
-Brian

 

[Drej]

It might be easier to apply the equivalent force, if you can convert the acceleration to force and be happy that the force calculated is the REAL force i.e. one that carries with it the appropriate participating mass. Converting acceleration time-history to displacement is fairly easy, you just need to integrate back twice (see the ANSYS int1 and int2 functions) using the following code (amend as necessary):

C******************************************************
C******************************************************
C***** NUMERICAL INTEGRATION OF A FUNCTION USING ******
c***** ANSYS APDL COMMANDS. REQUIRES TWO FILES ********
C***** TIME_AXIS.DAT and FUNC_AXIS.DAT, BOTH MUST *****
C***** BE WITHIN THE WORKING DIRECTORY WHICH **********
C***** INTEGRA.INP IS RUN. THE OUTPUT IS AN ***********
C***** INTEGRAL OF THE FUNCTION GIVEN IN **************
C***** FUNC_AXIS.DAT. CAN BE USED TO INTEGRATE ********
C***** TIME HISTORY (ACCELERATION ETC.) TO OBTAIN *****
C***** OTHER VARIABLES SUCH AS VELOCITY/DISPLACEMENT **
C******************************************************
C******************************************************
C******************************************************
C******************************************************
C**** MUST FIRST SET THE NUMBER OF DATA POINTS ********
C**** SEE THE "no_of_points" VARIABLE BELOW *************


fini
/cle

no_of_points=4096

*SET,XTIME
*SET,XFUNC
*SET,XINTE

*DIM,XTIME,,no_of_points
*DIM,XFUNC,,no_of_points
*DIM,XINTE,,no_of_points

*VREAD,XTIME(1),TIME_AXIS,dat,,1
(1f8.6)

*VREAD,XFUNC(1),FUNC_AXIS,dat,,1
(1f8.6)

C*** integrate

*VOPER,XINTE,XFUNC,INT1,XTIME

*VLEN,no_of_points
/output,OUTPUT_velocity,dat
*vwrite,XINTE(1)
(2f12.7)

/output

Converting acceleration-frequency to displacement-frequency is NOT easy, which is why using force is probably the preferred option.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com