ansys能算流动的流体作用下的结构振动及声辐射吗？
请问大侠：ansys能算流动的流体作用下的结构振动及声辐射吗？ 没做过这方面的分析不过应该是可以的，见过有人发表过相关方面的文章
另外我这里也有一个简单的例子
(Example of acoustic radiating sphere. Comparison w/ hand calculations. ）/com, Sample input file for acoustics
/com, Radiating sphere problem (simple case), compare w/ theory
/com,
!------------------------------------------------------------
! Check if running file in batch or interactive mode
! If batch mode, redirect plots to GRPH file
!------------------------------------------------------------
*get,STATGUI,active,,int
*if,STATGUI,eq,0,then
/show,file
*endif
!------------------------------------------------------------
! Define variables for problem:
! Radiating Sphere of Radius SPHRRADS with uniform surface
! velocity of VELOCITY oscillating at FREQUENC
!------------------------------------------------------------
*set,FREQUENC,3000
*set,VELOCITY,0.005
*set,PI ,acos(-1)
*set,SPHRRADS,0.1
!------------------------------------------------------------
! Fluid properties:
! Density, Speed of sound in water, Reference pressure
!------------------------------------------------------------
*set,WATRDENS,1000
*set,WATRSONC,1500
*set,REFEPRES,1e-6
!------------------------------------------------------------
! Geometry info
! Infinite radius at INFIRADS meters
! INFIXOFF, INFIYOFF not used right now...
!------------------------------------------------------------
*set,INFIRADS,5
*set,INFIXOFF,0.0
*set,INFIYOFF,0.0
!------------------------------------------------------------
! Mesh info
! Use mapped mesh? YES=1 NO=0 (use NO for now)
! Elements per wavelength (EPW)
!------------------------------------------------------------
*set,MAPDMESH,0
*set,TRIMESH ,1
*set,EPW ,15
!------------------------------------------------------------
! Graphics settings
! Set title and subtitles
! Make sure the legend is always on (/plopt,info,on)
! Put global triad at right top corner (/triad,rtop)
! Turn on Full Graphics because of DDTSREP#16215
!------------------------------------------------------------
/title,Uniformly Radiating Sphere, EPW=%EPW%
/stitle,1,Sphere radius of %SPHRRADS%m
/stitle,2,Frequency at %FREQUENC%Hz
/stitle,3,Uniform velocity of %VELOCITY%m/s
/stitle,4,Infinite Boundary of %INFIRADS%m at (%INFIXOFF%,%INFIYOFF%)
/plopt,info,on
/triad,rtop
/graphics,full
!------------------------------------------------------------
! Enter Preprocessor
!------------------------------------------------------------
/prep7
!------------------------------------------------------------
! Define elements
! 1 = fluid w/ structure
! 2 = fluid no structure
! 3 = infinite fluid
! Define elements and keyopts (et) (keyopt)
! Define real constants (r)
! Define material properties (mp)
!------------------------------------------------------------
et,1,fluid29
keyopt,1,2,0
keyopt,1,3,1
et,2,fluid29
keyopt,2,2,1
keyopt,2,3,1
et,3,fluid129
keyopt,3,3,1
r,1,REFEPRES
r,2,REFEPRES
r,3,INFIRADS,0,0,
mp,dens,1,WATRDENS
mp,sonc,1,WATRSONC
mp,dens,2,WATRDENS
mp,sonc,2,WATRSONC
mp,sonc,3,WATRSONC
!------------------------------------------------------------
! Create geometry
! Create five 90 degree quarter circles (pcirc)
! Merge keypoints (nummrg,kp)
!------------------------------------------------------------
pcirc,1,SPHRRADS,0,90,
pcirc,2,1,0,90,
pcirc,3,2,0,90,
pcirc,4,3,0,90,
pcirc,5,4,0,90,
nummrg,kp
!------------------------------------------------------------
! Mesh
! Set global element size based on EPW above
! Map with quads, quad-dominant for free mesh (mshape,0)
! Mesh mapped or free (mshkey)
! Set area attributes (aatt)
! Mesh all areas (amesh)
! Set plot controls based on element type number
!------------------------------------------------------------
esize,(WATRSONC/FREQUENC)/EPW
mshape,TRIMESH
mshkey,MAPDMESH
aatt,2,2,2
amesh,all
/pnum,type,1
/num,1
/auto
eplot
!------------------------------------------------------------
! Rotate all nodes in cylindrical CS
!------------------------------------------------------------
csys,1
nrotate,all
!------------------------------------------------------------
! Change elements near center to fluid with struct present
!------------------------------------------------------------
type,1
real,1
mat,1
nsel,s,loc,x,SPHRRADS
esln
nsle
emodif,all
!------------------------------------------------------------
! Apply struct boundary conditions on element type 1
! Constrain all translation DOF (the "free" DOF)
! Reapply velocity as displacement on inner nodes in radial dir. (ux)
! Apply FSI (fluid-struct interface) flag to active
!------------------------------------------------------------
d,all,uy
d,all,ux
nsel,s,loc,x,SPHRRADS
d,all,ux,0,-VELOCITY/(2*PI*FREQUENC)
sf,all,fsi
!------------------------------------------------------------
! Mesh Infinite fluid domain
! Instead of meshing, use ESURF to generate elements on existing mesh
!------------------------------------------------------------
type,3
real,3
mat,3
esel,all
nsel,s,loc,x,INFIRADS,INFIRADS+0.0001
esurf,all
allsel,all
finish
!------------------------------------------------------------
! solution options
! Full harmonic analysis
! frequency at FREQUENC
! select everything & solve
!------------------------------------------------------------
/solu
antype,harm
hropt,full
hrout,on
lumpm,0
!eqslv,front
eqslv,sparse
harfrq,FREQUENC
nsubst,
kbc,0
allsel,all
solve
finish
!------------------------------------------------------------
! postprocessing w/ annotations
! Load real (set,1,1,1,0) and plot pressure
! Load imag (set,1,1,1,1) and plot pressure
! do a load case comb. to SRSS for pressure magnitude
!------------------------------------------------------------
/post1
/tsp,,0.75
/ann,dele
/tla,-.90,.90,Plot of real part of pressure
/dscale,1,off
set,1,1,1,0
plnsol,pres
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
/tsp,,0.75
/ann,dele
/tla,-.90,.90,Plot of imag part of pressure
set,1,1,1,1
/replot
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
/tsp,,0.75
/ann,dele
/tla,-.90,.90,Plot of magnitude of pressure
lcdef,1,1,1,0
lcoper,srss,1
/replot
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
/ann,dele
!------------------------------------------------------------
! path operations
! this part gets ugly...
!------------------------------------------------------------
csys,0
lsel,s,loc,x,0
nsll,s,1
*get,NCOUNT,node,,count
csys,1
nsel,s,loc,x,SPHRRADS
nsel,r,loc,y,90,90.0001
STRTNODE=ndnext(0)
nsel,s,loc,x,INFIRADS,INFIRADS+0.0001
nsel,r,loc,y,90,90.0001
FININODE=ndnext(0)
allsel,all
path,RADIAL,2,30,(NCOUNT-1)
ppath,1,STRTNODE
ppath,2,FININODE
avprin,0,0,
set,1,1,1,0
pdef,REALPRES,pres,,noavg
set,1,1,1,1
pdef,IMAGPRES,pres,,noavg
!plpath,REALPRES,IMAGPRES
paget,tracpoin,poin
paget,tracdata,tabl
paget,traclabl,labe
*dim,RADSPATH,table,NCOUNT,7
*do,ICOUNT,1,NCOUNT
WAVENUMB=2*PI*FREQUENC/WATRSONC
CURRRADS=TRACDATA(ICOUNT,2,1)
TEMPAMPL=WATRDENS*WATRSONC*VELOCITY*WAVENUMB*(SPHRRADS**2)/CURRRADS
TEMPAMPL=TEMPAMPL/(1+(WAVENUMB*SPHRRADS)**2)
TEMPAMRC=WAVENUMB*SPHRRADS*cos(WAVENUMB*(CURRRADS-SPHRRADS))
TEMPAMRS=sin(WAVENUMB*(CURRRADS-SPHRRADS))
TEMPAMIC=cos(WAVENUMB*(CURRRADS-SPHRRADS))
TEMPAMIS=-WAVENUMB*SPHRRADS*sin(WAVENUMB*(CURRRADS-SPHRRADS))
RADSPATH(ICOUNT,1)=TRACDATA(ICOUNT,2,1)
RADSPATH(ICOUNT,2)=TRACDATA(ICOUNT,5,1)
RADSPATH(ICOUNT,3)=TEMPAMPL*(TEMPAMRC+TEMPAMRS)
RADSPATH(ICOUNT,4)=TRACDATA(ICOUNT,6,1)
RADSPATH(ICOUNT,5)=TEMPAMPL*(TEMPAMIC+TEMPAMIS)
RADSPATH(ICOUNT,6)=sqrt(TRACDATA(ICOUNT,5,1)**2+TRACDATA(ICOUNT,6,1)**2)
TEMP1 =TEMPAMPL*(TEMPAMRC+TEMPAMRS)
TEMP2 =TEMPAMPL*(TEMPAMIC+TEMPAMIS)
RADSPATH(ICOUNT,7)=sqrt(TEMP1**2+TEMP2**2)
*enddo
/gcolumn,1,ANSYS
/gcolumn,2,Theory
/axlab,x,Radial Distance
/axlab,y,Real Pressure (Pa)
*vplot,RADSPATH(1,1),RADSPATH(1,2),3
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
/axlab,y,Imaginary Pressure (Pa)
*vplot,RADSPATH(1,1),RADSPATH(1,4),5
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
/axlab,y,Magnitude of Pressure (Pa)
*vplot,RADSPATH(1,1),RADSPATH(1,6),7
*if,STATGUI,eq,2,then
*ask,Paused,Press Enter to Continue,'pause'
*endif
!parsav,all
finish
*del,TEMPAMPL
*del,TEMPAMRC
*del,TEMPAMRS
*del,TEMPAMIC
*del,TEMPAMIS
*del,TEMP1
*del,TEMP2
*del,CURRRADS
*del,WAVENUMB
!=(DENSITY*SPEED_OF_SOUND*VELOCITY*WAVE_NUMBER*RADIUS*(RADIUS/C2)/(1+(WAVE_NUMBER*RADIUS)^2))*(WAVE_NUMBER*RADIUS*COS(WAVE_NUMBER*(C2-RADIUS))+SIN(WAVE_NUMBER*(C2-RADIUS)))
!=(DENSITY*SPEED_OF_SOUND*VELOCITY*WAVE_NUMBER*RADIUS*(RADIUS/C2)/(1+(WAVE_NUMBER*RADIUS)^2))*(COS(WAVE_NUMBER*(C2-RADIUS))-WAVE_NUMBER*RADIUS*SIN(WAVE_NUMBER*(C2-RADIUS)))
*if,STATGUI,eq,0,then
/exit
*endif Acoustic Superelements
Q: Has anybody got superelements to work with fluid 29/30 (acoustic, pressure DOF) elements?
A: Yes, superelements work fine w/ acoustic elements, too. Useful for those nasty 3D models -- even w/ 2D radiation problems, it works fine and is helpful.
There are many "gotchas" when doing this, so be careful and start off with a simple model. For example, in the GEN pass, you shouldn't define any fluid29 w/ structure present (i.e., if you use top-down substructuring, null FLUID29 w/ structure present). Any model in the GEN pass containing unsymm elements uses that for the SE which means that only stiffness is stored, not mass. In other words:
You can have mass & stiffness (& damping) for symm matrices for SE or
You can have stiffness only for unsym matrices for SE part -- basically, trying to substructure FSI part is unusable for modal or harmonic.
However, in the USE pass, you can use unsymm matrices for non-SE portions (i.e., in the USE pass, define your FLUID29 with FSI). A simple modal analysis input file (acoustic_se.inp) is attached. I didn't spend much time on it, so it's not fancy, but I hope you get the idea.
Another one for those doing piezo is that VOLT and UX/UY/UZ can't be MDOF together, mainly because VOLT has no mass or damping equivalent. Instead of applying voltage as a load vector after the GEN pass, I usually do this as a non-SE element in the USE pass.
I've use a combination of superelements and non-superelements with pretty good success in modal and harmonic acoustic analyses. Like I mentioned above, there are some things which may not be intuitive, so try simple models first. Chop up your fluid domain into repeatable sections except for infinite boundary or FSI areas. Then, you can use SE in those areas (SETRAN, etc.). Make sure you have M not only at boundaries of SE but inside, too, since you need proper mass characterization (mass and damping are reduced via Guyan reduction which is approximate, instead of being exact like the stiffness matrix because stiffness can be directly condensed to a reduced matrix w/o problems -- damping and mass have time derivatives of DOF which make this very ugly, hence Guyan reduction is used instead for those terms).
Anyways, that's my two cents on the above. Like I mentioned above, it can be done, but be careful ofthe procedure andselecting MDOF. 回复 Chelsea 的帖子
先谢过了，我好好研究一下 回复 Chelsea 的帖子
我想算的是结构在湍流脉动压力作用下的振动与声辐射，不知道如何模拟，哪位大侠给点指导、建议或者资料啊，不知道ansys能算这样的流固声耦合吗？
页:
[1]