Modal analysis with loads

[izyk]

Hi
I dont know how to perform a modal analysis with loads. I'm trying to find modes frequencies of membrane under pressure but applying a pressure changes nothing, membrane still oscillate around zero deflection. I know that constant load doesn't change frequencies but later i want to apply an electrostatic pressure which changes modes frequencies.
Regards

 

[cbrn]

Hi,
load can affect modal results because of the "stress-stiffening" effect (e.g. tension on a piano wire).
However, the way to do this is conceptually the same in WB and Classical:
- first run a static analysis. In Classical, be sure to activate "calculate prestress" in the analysis options. In WB, choose "modal analysis" in the "further analysis" dropdown list.
- then, without exiting /Solution (in Classical), choose a "new analysis -> modal" and make sure to have the "use prestress data" activated. In WB, choose your previous static analysis from the dropdown list as the prestress condition for the modal analysis.

Regards

 

[izyk]

ok, it worked but i obtained results different from theory.
I'm simulating a circular membrane clamped on edge without damping, large deformation and stress stiffening. Such system can be expressed by following formula:
mw'' + Kw = P*S
where: m - mass, K - spring constant, P - external pressure, S - area
Since external pressure is constant the modes frequencies become constant. In theory for specific dimensions and material properties i got first mode frequency = 8.8991e+005. In ANSYS 8.8748E+05. But when i applied a pressure the frequency increased i.e. P=0.4bar f=0.88880E+06, P=4bar f=0.10103E+07.
Where is the difference beetween theory and ansys?

Here is the script:
-----------------------------------------------------
FINISH
/CLEAR

/FILNAME,memcir50shell,0
/CWD,'C:\temp\ANSYS'

!* membrane
Rad=150
Tm=5

b=30

/PREP7
ET,1,SHELL63
R,1,Tm

MP,EX,1,169e+9*1e-6
PRXY,1,0.0625
DENS,1,2330*1e-18

PCIRC,Rad, ,0,360,
LESIZE,ALL,,,b,-5

MSHAPE,0,2D
MSHKEY,1
AMESH,ALL

!* applying loads and BC
FLST,5,4,4,ORDE,2
FITEM,5,1
FITEM,5,-4
LSEL,S, , ,P51X
NSLL,S,1

D,ALL,UX,0
D,ALL,UY,0
D,ALL,UZ,0
D,ALL,ROTX,0
D,ALL,ROTY,0
D,ALL,ROTZ,0

ALLSEL,ALL

SFA,1,1,pres,40000*1E-6

/SOLU
ANTYPE,STATIC
PSTRES,ON
NLGEOM,OFF
SSTIF,OFF

SOLVE
FINISH

/SOLU
ANTYPE,MODAL

UPCOORD,1.0,ON
PSTRES,ON

MODOPT,SUBSP,5
EQSLV,FRONT
LUMPM,0
MODOPT,SUBSP,5,0,0, ,OFF
RIGID,
SUBOPT,8,4,9,0,0,ALL

SOLVE
FINISH

save,memcir50shell,db
fini

 

[cbrn]

Hi,
the difference is that the K terms depend upon P, i.e. Kij = fij(P). In addition, you say you wanted large displacements and stress-stiffening, but the script shows that both are OFF (by the way: are you sure you do need Large Displacements? L.D. at 500 [kHz] should require an enormous amount of energy!).
In other terms, I think you are comparing FE and handcalc results with two different formulations, one less complete (handcalc) than the other, and there is a little confusion between what you did and what you wanted to do ;-) !

Regards

 

[izyk]

Ok, i didn;t know that for plates K depends upon P.
But now i can't receive results for electrostatic pressure. Because of unsymmetrical matrices i have to use unsymmetric extraction method. But it gives no results in results summary. The same for a membrane without load.
p.s. i don't want LD


------------------------------
FINISH
/CLEAR
/CWD,'C:\temp\ansys'

!* membrane
Rad=150
Tm=5
!* membrane_division
b=30

!* electrode_distance
h=-1
dif=20

!* voltage
v=5

/PREP7
ET,1,SHELL63
R,1,Tm
ET,2,TRANS126

MP,EX,1,130e+9*1e-6
MP,DENS,1,2330*1e-18
MP,PRXY,1,0.278

WPOFFS,0,0,dif
PCIRC,Rad, ,0,360,
WPOFFS,0,0,-dif

LESIZE,ALL,,,b

TYPE,1
MSHAPE,0,2D
MSHKEY,1
AMESH,ALL

!* transducer

NSEL,S,LOC,Z,dif
CM,tr,NODE
ALLSEL,ALL
EMTGEN,'tr','EMTELM','EMTPNO','UZ',h,0,1E-02,0.8854E-05

NSEL,S,LOC,Z,dif+h
D,ALL,,0,,,,UZ
D,ALL,VOLT,v

CMSEL,S,TR
D,ALL,VOLT,0

!* applying loads and BC
FLST,5,4,4,ORDE,2
FITEM,5,1
FITEM,5,-4
LSEL,S, , ,P51X
NSLL,S,1

D,ALL,UX,0
D,ALL,UY,0
D,ALL,UZ,0
D,ALL,ROTX,0
D,ALL,ROTY,0
D,ALL,ROTZ,0

ALLSEL,ALL

FINISH

/SOLU
ANTYPE,STATIC
PSTRES,ON
NLGEOM,OFF
SSTIF,OFF

SOLVE
FINISH

/SOLU
ANTYPE,MODAL
UPCOORD,1.0,ON
PSTRES,ON

MODOPT,UNSYM,5
EQSLV,FRONT
LUMPM,0
MODOPT,UNSYM,5,0,0, ,OFF
RIGID,
SUBOPT,8,4,9,0,0,ALL

SOLVE
FINISH

fini