【转帖】Piezoelectric - 压电材料振动能量采集的有限元分析
Piezoelectric - 压电材料振动能量采集的有限元分析!1) Initialisation of elements and material properties
/TITLE, Piezoelectric Vibration Energy Harvester
/UNITS,MKS
accelx=0 !Acceleration in X
accely=0 !Acceleration in Y
accelz=2.5 !Acceleration in Z
/COM,
/COM, Finite Element Model of a Piezoelectric Energy Harvester
/COM,
/PREP7
/COM,Define Element Types Used During FEA Analysis
ET,1,SOLID5,0 !8-Node Coupled Field Piezoelectric Element For PZT
ET,2,SOLID45 !8-Node Solid Element For Modelling Tungsten Mass and
!steel Shim
ET,3,SHELL41 !4-Node Membrane Shell Element (Electrode), Not used in
!this project
ET,4,TARGE170,0 !3D Target surface for modelling bonding contact
!between tungsten mass and beam
ET,5,CONTA174 !Coupled field contact surface for modelling contact
!between tungsten mass and beam
/COM,Define Element Type Used During Electrical Analysis
ET,6,CIRCU94,0 !Define Resistor
/COM, !Define Keyopts for Finite Elements
KEYOPT,4,5,1 !Set TARGE 170 to solid-solid constraint
KEYOPT,5,1,0 !UX,UY,UZ
KEYOPT,5,2,2 !Contact algorithm: MPC
KEYOPT,5,4,1 !Contact detection on nodal point
KEYOPT,5,5,0 !No automated contact adjustment
KEYOPT,5,7,0 !No element level time increment control
KEYOPT,5,8,0 !No asymmetric contact selection
KEYOPT,5,9,1 !Exclude both initial geometrical penetration or gap
!and offset
KEYOPT,5,10,1 !Update contact stiffness each substep based on mean stress
!of underlying elements
KEYOPT,5,12,5 !Bonded always contact behaviour
/COM,ZT-SH4 (Navy Type VI) Material Properties
/COM,iezo Systems Inc.
EMUNIT, MKS ! Free space permittivity
MP,DENS,1,7500 !Material density
MP,PERX,1,3130 !Relative permittivity MP,PERY,1,3130
MP,PERZ,1,3400
TB,ANEL,1,1,,1 !Flexibility matrix - inverted by Ansys
TBDATA,1,16.5e-12,-4.78e-12,-8.45e-12
TBDATA,7,16.5e-12,-8.45e-12
TBDATA,12,20.7e-12
TBDATA,16,43.5e-12
TBDATA,19,43.5e-12
TBDATA,21,42.6e-12
TB,PIEZ,1 ! Piezoelectric constant matrix
TBDATA,3,-6.622
TBDATA,6,-6.622
TBDATA,9,23.24
TBDATA,11,17.034
TBDATA,13,17.394
MP,MURX,1,0 !False material properties to suppress error messages
MP,KXX,1,0
/COM,Steel Shim Material Properties
MP,DENS,2,7700 !Density
MP,EX,2,207e9 !Young's Modulus
MP,PRXY,2,0.3 !Poisson's ratio
!MP,RSVX,2,72e-8!Resistivity (Volt DOF will be coupled later)
/COM,Tungsten Mass Material Properties
MP,DENS,3,17000 !Density
MP,EX,3,540e9 !Mass deformation will be negligible
MP,PRXY,3,0.28 !Poisson's ratio
/COM,Nickel Electrode Material Properties, not used in this
/COM,project
R,1,0.2e-6 !Thickness of top nickel electrode
R,2,0.2e-6 !Thickness of bottom nickel electrode
MP,EX,4,207e9 !Young's Modulus
MP,PRXY,4,0.3 !Poisson's ratio
/COM,Contact material properties
REAL,3 !Set element real constant attribute pointer
R,3,,,,,,
RMORE,,,,,,
RMORE,,0,,,,
RMORE,0 !Set electrical contact conductance
ALLSEL,ALL,ALL !Select all entities
/COM,Define real constants for circuit elements
R,4,180e3 !Define Resistor Properties (Defaults)
!Application of material properties to solid geometry
/COM,Apply material properties to volumes of imported
/COM,ro/Engineer Wildfire 2 IGES model
VSEL,S,VOLU,,2,,,0!Select volume 2 (Bottom Piezo layer)
VSEL,A,VOLU,,3,,,0!Additionally select volume 3 (Top Piezo layer)
VATT,1,1,1,0 !Apply PZT-5144 material properties
VSEL,S,VOLU,,1,,,0!Select volume 1(Steel centre shim)
VATT,2,1,2,0 !Apply steel material properties
VSEL,S,VOLU,,4,,,0!Select volume 4 (Tungsten mass)
VATT,3,1,2,0 !Apply tungsten material properties
/COM,Set mesh densities
/COM,ZT thickness density
LSEL,S,LINE,,38,,,0!Select bottom PZT layer thickness
LSEL,A,LINE,,84,,,0!Select top PZT layer thickness
LESIZE,ALL,,,3 !Specify 3 divisions mesh density
/COM,Steel shim thickness density
LSEL,S,LINE,,12,,,0
LESIZE,Al1,,,2 !Specify 2 divisions mesh density
/COMBeam width density
LSEL,S,LINE,,4,,,0
LSEL,A,LINE,,10,,,0
LSEL,A,LINE,,41,,,0
LESIZE,ALL,,,4 !4 divisions mesh density
/COM,Beam length density
LSEL,S,LINE,,2,,,0
LSEL,A,LINE,,9,,,O
LSEL,A,LINE,,81,,,0
LESIZE,ALL,,,120! 120 divisions mesh density
/COM,Tungsten mass mesh density
LSEL,S,LINE,,109
LESIZE,ALL,,,3
LSEL,S,LINE,,111,,,0
LESIZE,ALL,,,2
LSEL,S,LINE,,110,,,0
LESIZE,ALL,,,4
/COM,Mesh all volumes and areas
MSHKEY,1 !Set mapped mesh
ALLSEL,ALL,VOLU !Select all volumes to be meshed
VMESH,ALL !Mesh all volumes
!Coupling DOF
!The VOLT DOF is coupled between the dielectric and
!conductive layers in the model. This procedure uses the CP command to couple the
!DOF set of the nodes in the selected region, hence, the procedure must be performed after
!meshing.
/COM,Couple voltage degree of freedom between layers
ASEL,S,AREA,,41,,,0!Select top electrode
NSLA,S,1 !Select nodes related to top electrode
NSEL,U,LOC,X,10.7e-3,30e-3
CM,top_electrode,NODE !Create component from nodes
ASEL,S,AREA,,34,,,0!Select bottom electrode
NSLA,S,1 !Select nodes related to top electrode
NSEL,U,LOC,X,10.7e-3,30e-3
CM,bottom_electrode,NODE!Create component from nodes
NSEL,S,NODE,,top_electrode
NSEL,A,NODE,,bottom_electrode
CP,I,VOLT,ALL !Couple voltage degree of freedom for all nodes
*GET,OUT ELECT,NODE,O,NUM,MIN !Get master node on top electrode
VSEL,S,VOLU,,1,,,1!Select centre shim
NSLV,S,1 !Select nodes associated with volume
CM,centre shim,NODE !Create component from nodes
CP,NEXT,VOLT,ALL !Couple voltage degree of freedom for all nodes
*GET,NCENTRE,NODE,O,NUM,MIN !Get master centre electrode node
ALLSEL
!D.1.5 Modelling contact of proof mass
!In this section of the analysis, a target element is defined on the base of the tungsten
!mass and a contactelement is defined on the top surface of the beam as described in ANSYS
!Inc. (2004d).
ASEL,S,AREA,,48,,,0 !Select bottom of tungsten mass
NSLA,S,1 !Select nodes related to top electrode
CM,target_surface,NODE !Create component from nodes
ALLSEL,ALL,ALL !Select all entities
/COM,Define contact pair's
NSEL,S,,,target_surface !Select nodes on base of tungsten mass
TYPE,4 ! Set target element
ESLN,S,0 !Select elements attached to nodes
ESURF,ALL !Create target elements
ASEL,S,AREA,,41,,,0!Select top electrode
NSLA,S,1 !Select nodes related to top electrode
TYPE,5 !Set contact element type
ESLN,S,0 !Select elements attached to nodes
ESURF,ALL !Create contact elements
ALLSEL!Select all
FINISH
!2) Analysis
!2.1) Static analysis
/COM,Static analysis to test regime
/SOLU !Enter solution pre-processor
/COM,Apply boundary conditions
/COMCompletely rigid fixture, constrained Y for all
NSEL,S,LOC,X,0 !Select nodes at fixture location
D,ALL,UX,0,,,,UY,UZ, !Constrain all DOF
/COM,Define Model symmetry
NSEL,S,LOC,Y,0 !Select nodes at model symmetry line
DSYM,SYMM,Y !Apply symmetry boundary conditions
ALLSELL,ALL,ALL !Select all entities
/COM,Apply 5V to top and bottom electrode, OV to shim
D,top_electrode,VOLT,5
D,bottom_electrode,VOLT,5
D,centre_shim,VOLT,0
ALLSELL,ALL,ALL !Select all entities
ANTYPE,STATIC
SOLVE
FINISH
!2.2) Modal analysis
/COMModal analysis for determining resonance response of
/COM,harvester
/SOLU
/COM,Delete DOF from static analysis
DDELE,top_electrode,VOLT
DDELE,bottom_electrode,VOLT
ANTYPE,MODAL !Modal analysis
MODOPT,REDUC,8 !4 modes using reduced method
MXPAND,8 !Expand a114 modes
TOTAL,10,1
ALLSEL
D,NCENTRE,VOLT,0.0 !Ground centre electrode
DMPRAT,0.031 !Constant damping ratio
NSEL,ALL !Select all nodes
SOLVE !Solve current load step
FINISH
!2.3) Harmonic analysis without resistor
/COM,Haitnonic analysis around first resonant frequency
/SOLU
ANTYP,HARM !Set harmonic analysis
HARFRQ,30,120 !Set frequency range
NSUBST,36 !Set 2.5 Hz increments
KBC,1 !Loads step changed
D,NCENTRE,VOLT,0.0 !Ground centre electrode
DMPRAT,0.031 !Constant damping ratio
ALLSEL
ACEL,accelx,accely,accelz !Set accelerations
SOLVE
FINISH
/POST26
NSOL,9, OUT_ELECT, VOLT,,output_voltage ! Store output power
FINISH
!2.4) Harmonic analysis with resistor
/COM,Harmonic analysis around first frequency with
/COM,resistance load
/COM,Create circuit geometry
/PREP7
N,,0,-5e-3,0, !Defines node 1 for circuit
N,,5e-3,-5e-3,0,!Defines node 2 for circuit
/COM,Create circuit elements on geometry
TYPE,6 !Set circuit element type (Resistor)
REAL,4 !Set circuit element constants (Resistance)
E,5505,5506 !Plot Resistor
/ICSCALE,1,0.1 !Scale circuit elements to correct size
/COM,Couple voltage degrees of freedom between circuit
/COM,and FE model. Places resistor between top and bottom
/COM electrode
NSEL,S,NODE,,5505!Select input node in circuit
CP,1,VOLT,ALL !Couple voltage Degree of Freedom on top elect
NSEL,S,NODE,,5506!Select input node in circuit
CP,4,VOLT,ALL !Couple voltage Degree of Freedom on centre elect
ALLSELL,ALL,ALL !Select all entities
FINISH
/COM,Harmonic analysis with resistor coupled to outer electrodes
/SOLU
ANTYP,HARM !Set harmonic analysis
/COMSet constraints on DOF
NSEL,S,LOC,X,0 !Select nodes at fixture location
D,ALL,UX,O,,,,UY,UZ, !Constrain all DOF
/COMDefine Model symmetry
NSEL,S,LOC,Y,0 !Select nodes at model symmetry line
DSYM,SYMM,Y !Apply symmetry boundary conditions
ALLSELL,ALL,ALL !Select all entities
HARFRQ,30,120 !Set frequency range
NSUBST,36 !Set 2.5 Hz increments
KBC,1 !Loads step changed
D,NCENTRE,VOLT,0.0 !Ground centre electrode
DMPRAT,0.031 !Constant damping ratio
ALLSEL
ACEL,accelx,accely,accelz !Set accelerations
SOLVE
FINISH
!2.5) Spectral Analysis
/COM,Spectral analysis
/SOLU
ALLSEL
DDELE,ALL,ALL !Delete all previous constraints
ACEL,0,0,0 !Set accelerations to zero (zero gravity)
D,NCENTRE,VOLT,0.0 !Ground centre electrode
NSEL,S,LOC,X,0 !Select nodes at fixture location
D,ALL,UX,0,,,,UY,UZ, !Constrain all DOF
/COM,Define Model symmetry
NSEL,S,LOC,Y,0 !Select nodes at model symmetry line
DSYM,SYMM,Y !Apply symmetry boundary conditions
ALLSELL,ALL,ALL !Select all entities
/COM,Modal analysis
/SOLU
ANTYPE,MODAL ! Mode-frequency analysis
MODOPT,REDUC,,,,4 ! Householder, print first 3 reduced mode shapes
MXPAND,4, ! Expand first mode shape
TOTAL,10,1
OUTPR,BASIC,1
SOLVE
FINISH
/COM,Spectrum Analysis
/SOLU
ANTYPE,SPECTR ! Spectrum analysis
SPOPT,SPRS ! Single point spectrum
DMPRAT,0.031 !Constant damping ratio
SED,0,0,1 ! Global Z-axis as spectrum direction
SVTYPE,2 ! Seismic acceleration spectrum
MCOMB,SRSS,0.001,
/COMDefine frequency table (from table 4.1)
FREQ,12,31,32,34,35,57,59,67,68 !Frequency points 1-9 (Hz)
FREQ,69,70,72,73! Frequency 10-13 (Hz)
/COM,Define acceleration table to match frequency table (from
/COM,table 4.1)
SV,0.031,0.167,0.052,0.067,0.067,0.059,0.168,0.054,0.072,0.284
SV,0.031,0.078,0.078,0.068,0.07 ! Acceleration magnitudes (m/s2)
OUTRES,ALL,ALL, !Output all results to file
ALLSEL
SOLVE
FINISH
/Post26 !Enter post processing
/INPUT,,mcom,,1,0 !Input combined modes results file
FINISH 一秒时间历程的瞬态分析： 电压：; \
瞬态分析的独立程序如下：
/PREP7
RESUME,PZT_geo,db,,0,0
!D.1.1 Initialisation of elements and material properties
/UNITS,MKS
/COM,
/COM, Finite Element Model of a Piezoelectric Energy Harvester
/COM,
/PREP7
/COM, Define Element Types Used During FEA Analysis
ET,1,SOLID5,0 !8-Node Coupled Field Piezoelectric Element For PZT
ET,2,SOLID45 !8-Node Solid Element For Modelling Tungsten Mass and
!steel Shim
ET,3,SHELL41 !4-Node Membrane Shell Element (Electrode), Not used in
!this project
ET,4,TARGE170,0 !3D Target surface for modelling bonding contact
!between tungsten mass and beam
ET,5,CONTA174 !Coupled field contact surface for modelling contact
!between tungsten mass and beam
/COM,Define Element Type Used During Electrical Analysis
ET,6,CIRCU94,0 !Define Resistor
/COM, !Define Keyopts for Finite Elements
KEYOPT,4,5,1 !Set TARGE 170 to solid-solid constraint
KEYOPT,5,1,0 !UX,UY,UZ
KEYOPT,5,2,2 !Contact algorithm: MPC
KEYOPT,5,4,1 !Contact detection on nodal point
KEYOPT,5,5,0 !No automated contact adjustment
KEYOPT,5,7,0 !No element level time increment control
KEYOPT,5,8,0 !No asymmetric contact selection
KEYOPT,5,9,1 !Exclude both initial geometrical penetration or gap
!and offset
KEYOPT,5,10,1 !Update contact stiffness each substep based on mean stress
!of underlying elements
KEYOPT,5,12,5 !Bonded always contact behaviour
/COMZT-SH4 (Navy Type VI) Material Properties
/COM,iezo Systems Inc.
EMUNIT, MKS ! Free space permittivity
MP,DENS,1,7500 !Material density
MP,PERX,1,3130 !Relative permittivity MP,PERY,1,3130
MP,PERZ,1,3400
TB,ANEL,1,1,,1 !Flexibility matrix - inverted by Ansys
TBDATA,1,16.5e-12,-4.78e-12,-8.45e-12
TBDATA,7,16.5e-12,-8.45e-12
TBDATA,12,20.7e-12
TBDATA,16,43.5e-12
TBDATA,19,43.5e-12
TBDATA,21,42.6e-12
TB,PIEZ,1 ! Piezoelectric constant matrix
TBDATA,3,-6.622
TBDATA,6,-6.622
TBDATA,9,23.24
TBDATA,11,17.034
TBDATA,13,17.394
MP,MURX,1,0 !False material properties to suppress error messages
MP,KXX,1,0
/COM,Steel Shim Material Properties
MP,DENS,2,7700 !Density
MP,EX,2,207e9 !Young's Modulus
MP,PRXY,2,0.3 !Poisson's ratio
!MP,RSVX,2,72e-8!Resistivity (Volt DOF will be coupled later)
/COM,Tungsten Mass Material Properties
MP,DENS,3,17000 !Density
MP,EX,3,540e9 !Mass deformation will be negligible
MP,PRXY,3,0.28 !Poisson's ratio
/COMNickel Electrode Material Properties, not used in this
/COM,project
R,1,0.2e-6 !Thickness of top nickel electrode
R,2,0.2e-6 !Thickness of bottom nickel electrode
MP,EX,4,207e9 !Young's Modulus
MP,PRXY,4,0.3 !Poisson's ratio
/COM,Contact material properties
REAL,3 !Set element real constant attribute pointer
R,3,,,,,,
RMORE,,,,,,
RMORE,,0,,,,
RMORE,0 !Set electrical contact conductance
ALLSEL,ALL,ALL !Select all entities
/COM,Define real constants for circuit elements
R,4,180e3 !Define Resistor Properties (Defaults)
/COM,Apply material properties to volumes of imported
/COM,ro/Engineer Wildfire 2 IGES model
VSEL,S,VOLU,,1,,,0!Select volume 2 (Bottom Piezo layer)
VSEL,A,VOLU,,3,,,0!Additionally select volume 3 (Top Piezo layer)
VATT,1,1,1,0 !Apply PZT-5144 material properties
VSEL,S,VOLU,,2,,,0!Select volume 1(Steel centre shim)
VATT,2,1,2,0 !Apply steel material properties
VSEL,S,VOLU,,4,,,0!Select volume 4 (Tungsten mass)
VATT,3,1,2,0 !Apply tungsten material properties
/COM,Set mesh densities
/COM,ZT thickness density
LSEL,S,LINE,,10,,,0!Select bottom PZT layer thickness
LSEL,A,LINE,,26,,,0!Select top PZT layer thickness
LESIZE,ALL,,,3 !Specify 3 divisions mesh density
/COM,Steel shim thickness density
LSEL,S,LINE,,18,,,0
LESIZE,Al1,,,2 !Specify 2 divisions mesh density
/COMBeam width density
LSEL,S,LINE,,1,,,0
LSEL,A,LINE,,5,,,0
LSEL,A,LINE,,13,,,0
LESIZE,ALL,,,4 !4 divisions mesh density
/COM,Beam length density
LSEL,S,LINE,,2,,,0
LSEL,A,LINE,,6,,,O
LSEL,A,LINE,,14,,,0
LESIZE,ALL,,,120! 120 divisions mesh density
/COM,Tungsten mass mesh density
LSEL,S,LINE,,38
LESIZE,ALL,,,3
LSEL,S,LINE,,33,,,0
LESIZE,ALL,,,2
LSEL,S,LINE,,34,,,0
LESIZE,ALL,,,4
/COM,Mesh all volumes and areas
MSHKEY,1 !Set mapped mesh
ALLSEL,ALL,VOLU !Select all volumes to be meshed
VMESH,ALL !Mesh all volumes
/COM,Couple voltage degree of freedom between layers
ASEL,S,AREA,,12,,,0!Select top electrode
NSLA,S,1 !Select nodes related to top_electrode
NSEL,U,LOC,X,10.7e-3,30e-3
CM,top_electrode,NODE !Create component from nodes
ASEL,S,AREA,,1,,,0!Select bottom electrode
NSLA,S,1 !Select nodes related to top_electrode
NSEL,U,LOC,X,10.7e-3,30e-3
CM,bottom_electrode,NODE!Create component from nodes
NSEL,S,NODE,,top_electrode
NSEL,A,NODE,,bottom_electrode
CP,1,VOLT,ALL !Couple voltage degree of freedom for all nodes
*GET,OUT_ELECT,NODE,0,NUM,MIN !Get master node on top_electrode
VSEL,S, , , 2
!VSEL,S,VOLU,,2,,,1!Select centre shim
NSLV,S,1 !Select nodes associated with volume
CM,centre_shim,NODE !Create component from nodes
CP,NEXT,VOLT,ALL !Couple voltage degree of freedom for all nodes
*GET,NCENTRE,NODE,0,NUM,MIN !Get master centre electrode node
ALLSEL
ASEL,S,AREA,,17,,,0 !Select bottom of tungsten mass
NSLA,S,1 !Select nodes related to top electrode
CM,target_surface,NODE !Create component from nodes
ALLSEL,ALL,ALL !Select all entities
/COM,Define contact pair's
NSEL,S,,,target_surface !Select nodes on base of tungsten mass
TYPE,4 ! Set target element
ESLN,S,0 !Select elements attached to nodes
ESURF,ALL !Create target elements
ASEL,S,AREA,,12,,,0!Select top electrode
NSLA,S,1 !Select nodes related to top electrode
TYPE,5 !Set contact element type
ESLN,S,0 !Select elements attached to nodes
ESURF,ALL !Create contact elements
ALLSEL!Select all
FINISH
CSYS,0
/SOLU !Enter solution pre-processor
NSEL,S,LOC,X,0 !Select nodes at fixture location
D,ALL,UX,0,,,,UY,UZ, !Constrain all DOF
ALLSELL,ALL,ALL !Select all entities
!*
NT=100
DT=0.01 !time increment
*dim,ac,,NT
/input,vibration_in,txt
!*
/SOLU
NSUBST,1, , ,1
OUTRES,ALL,1 !output result of each substep
ANTYPE,TRANS !transient
TINTP,,0.25,0.5,0.5,0.5,0,,,,,,
*do,i,1,NT
ACEL,0,0,ac(i)
TIME,i*DT
solve
*enddo
!*
/POST26
NSOL,2,6069,U,Z,
/GRID,1
PLVAR,2
震动波 部分GUI结果： 谢谢楼主{:{39}:} 请问这个材料是从学术会议的报告中摘出来的么？ 几何模型建立的程序没有
页:
[1]