×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Modal analysis with loads

Modal analysis with loads

Modal analysis with loads

(OP)
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

RE: Modal analysis with loads

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

RE: Modal analysis with loads

(OP)
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


 

RE: Modal analysis with loads

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 winky smile !

Regards

RE: Modal analysis with loads

(OP)
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
 

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources