本文摘要(由AI生成):
本文主要介绍了一个热/结构预载荷综合作用的悬臂梁案例。首先使用SOLID70进行稳态传热分析,然后使用SOLID185进行隐式预加载荷求解,接着将单元转换成SOLID164进行应力初始化,最后在瞬态阶段逐步增大压力。其中,SOLID70用于稳态的传热分析,SOLID185用于隐式预加载荷求解,SOLID164用于应力初始化。在瞬态阶段,使用ANSYS MULTIPHYSICS ls-dyna模块进行求解。
热/结构预载荷综合作用于一个悬臂梁,首先用SOLID70做热分析,然后将这个单元转换成SOLID185,并且将温度读入结构模型,再加上压力,进行隐式预加载荷求解。紧接着将单元转换成SOLID164,并且对这个的预荷模型进行应力初始化,最后在瞬态阶段逐步增大压力,在这里需要的输入文件为preload.inp。
fini
/clear
/title, Applying a Thermal/Structural Preload (preload.inp)
! Units: kilogram, meter, second, Newton, Pascal, Joule, Watt
! = = = = = = = = = = = = =先进行热分析【SOLID70用于稳态的传热分析,给梁的左侧施加热3,000 W/m3的热生成率,梁的右侧施以30 W/m2-℃界面散热系数(TBULK = 0℃),从梁的左侧(热)到右侧(冷)的热梯度为20℃ 】
/filnam,thermal,1
/title, ANSYS Heat Transfer Analysis
/prep7
et,1,SOLID70 ! thermal brick element
r,1 ! dummy real constant set
! Temperature-independent thermal material properties:
mp,dens,1,8.03e3 ! kg/m^3
mp,kxx,1,16.3 ! W/m-C
mp,c,1,502.0 ! J/kg-C
block,0,1,0,1,0,11
esize,0.25
vmesh,all
cm,nbeam,node !定义所有节点的组元
cm,ebeam,elem
fini
/solu
antype,static ! steady state heat transfer ****ysis
time,1.0
nsel,s,loc,x,0 ! left side of beam选择x=0的节点
Esln !选择节点对应的单元
bf,all,hgen,3.0e3 ! 3,000 W/m^3 heat generation on left side热生成载荷
esel,all
nsel,s,ext ! exterior beam nodes选择所有外部节点
nsel,r,loc,x,1.0 ! right side of beam再次选择x=1的节点
sf,all,conv,30.0,0.0 ! hf=30.0 W/m^2-C and Tbulk=0 degrees C施加对流
nsel,all
save
solve
fini
/post1
set,last
plnsol,temp!显示温度
/wait,5 !推迟5秒钟再读取下一个命令(5秒钟来显示温度)
save
fin
! = = = = = = = = = = = = =下面进行热应力分析【SOLID185单元用在热/结构隐式预加载荷分析,统一用缩减积分,基于温度的线性材料限定在0℃和500℃。所有的实际温度在这两个值之间,LDREAD用于读稳态的热传导的温度,1.1e5 N/m2压力 施加的梁的上部,在端给以自由度约束】
/filnam,preload,1
/title, ANSYS Implicit Static Preload Analysis
/prep7
bfdele,all,all ! remove thermal body force (heat generation) loads体载荷删除
sfdele,all,all ! remove thermal surface (convection) loads面载荷删除
/psf,pres,norm,2 !显示面载荷,查看有无没删除的
/dscale,,1.0 !设置位移显示的位移倍数
Eplot !显示单元
et,2,SOLID185 ! desired structural brick element
emodif,all,type,2 ! ETCHG,TTS creates SOLID45 elements单元修改
etdele,1 ! remove thermal bricks删除热单元
numcmp,type ! compress element type numbers 压缩单元号
keyopt,1,2,1 ! uniform reduced integration to match SOLID164统一降低整合,以匹配SOLID164
! Temperature-dependent structural properties
mp,dens,1, 8.03e3 ! kg/m^3 (canNOT be temp-dependent)
mptemp, 1, 0.0, 500.0 ! degrees C, two temperatures 2个温度0和500,对应不同材料参数
mpdata, ex,1,1,193.0e9,93.0e9 ! N/m^2 (temperature-dependent)
mpdata,nuxy,1,1,0.29,0.28 ! unitless (temperature-dependent)
mpdata,alpx,1,1,18.0e-6,16.0e-6 ! m/m-C (temperature-dependent)
! Note: Do not define plasticity in this ANSYS implicit preload
! ****ysis, since implicit-to-explicit sequential solutions
! assume linear elastic material properties and **all strain.
! Plasticity can be added in the subsequent transient run.
mplist,all,all !Lists linear material properties
fini
/solu
antype,static ! thermal strain (preload) structural ****ysis
time,1.0
nsubst,2,1000,2 !子步数
outres,all,last !输出
Ldread,temp,last,,,,thermal,rth ! temperature body loads (overwrites TUNIF),Reads results from the results file and applies them as loads初始温度
tref,0.0 ! reference temperature for "instantaneous" alpha参考温度
bflist,all,temp !List所有温度
nsel,s,loc,y,1 !y=1的节点
cm,nbeamtop,node !组元
Esln !单元
cm,ebeamtop,elem !单元组元【dyna中进行压力加载】
sf,all,press,1.1e5 ! apply pressure load (N/m^2) to top of beam单元上施加压力载荷
nsel,s,loc,z,0
d,all,uz,0.0 ! restrain aft end of beam约束z=0的作用节点的uz自由度
nsel,s,loc,z,0
nsel,r,loc,y,0.5 !z=0且y=0.5的节点
d,all,uy,0
nsel,s,loc,z,0
nsel,r,loc,x,0.5
d,all,ux,0
nsel,all
esel,all
save
solve
fini
/post1
set,last
/dscale,,10 ! exaggerate displacement
plnsol,s,eqv,2
/wait,5
! Note: Make sure that the yield stress is not exceeded, since
! the preload needs to have a linear response for the
! subsequent dynamic relaxation ****ysis
save
fini
! = = = = = = = = = = =下面进行显式分析 【SOLID185单元转化成SOLID164单元,添加0℃ 和500℃之间随温度变化的塑性(TB, BISO)材料性质,隐式求解的位移结果写入drelax文件(REXPORT),对指定的结果进行应力初始化(EDDRELAX, ANSYS),压力从预载的数值开始逐步提高,导致结构产生塑性变形,相同的温度会自动地写入dynamic.K输入文件】
/filnam,dynamic,1
/title, ANSYS/LS-DYNA Dynamic Relaxation and Transient Analyses
/psf,pres,norm,2 !显示面载荷,确认还没删除
/dscale,,1.0
/prep7
sfdele,all,all ! remove structural surface (pressure) loads删除面载荷(压力),约束保持
etchg,ite ! convert SOLID185 elements into SOLID164 elements转换单元
! Add plasticity to temperature-dependent properties定义温度相关的塑形材料
tb,biso,1,2 ! temperature-dependent BISO (2个温度)
tbtemp,0.0 ! first temperature
tbdata,1,66.7e6 ! N/m^2, yield stress at 0 degrees
tbdata,2,1.93e9 ! N/m^2, tangent modulus at 0 degrees
tbtemp,500.0 ! second temperature
tbdata,1,60.0e6 ! N/m^2, yield stress at 500 degrees
tbdata,2,0.93e9 ! N/m^2, tangent modulus at 500 degrees
! Note: Be sure to define a temperature range that exceeds the
! actual resulting temperatures. In this particular case,
! LS-DYNA will expect all temperatures to be between 0 and
! 500 degrees C. This requirement is on the LS-DYNA side.
edmp,hgls,1,5 !为显示动力学定义材料属性add hourglass control (1为材料号,5为沙漏类型)
edpart,create ! create part list
eddamp,all,,0.10 ! mass (alpha) damping
eddamp,1,,1.0e-6 ! stiffness (beta) damping
mplist,all,all !list材料
tblist,all,all !Lists the materialdata tables
fini
/solu
time,0.2 ! termination time (seconds)
rexport,dyna,,,,,preload,rst ! create drelax file,Exports displacements from an implicit run to ANSYSLS-DYNA,即dyna的初始位移使用隐士的位移结果。【Main Menu>Preprocessor>LS-DYNA Options>Constraints>Read Disp】
! Note: The temperatures written to the drelax file are NOT used by
! LS-DYNA to establish the thermal preload condition. Instead,
! the temperatures written via the *LOAD_THERMAL_CONSTANT_NODE
! command are used. The latter are stored in the ANSYS database
! as body force BF loads from the LDREAD command. These thermal
! loads remain active unless deleted (BFDELE,ALL,TEMP).
bflist,all,temp ! no need to re-issue LDREAD command【Lists the body force loads on nodes】
eddrelax,ansys ! stress initialization to a prescribed geometry【激活初始化到规定的几何形状或动态放松的显式分析】(Main Menu>Solution>Analysis Options>Dynamic Relax)【根据ANSYS(隐式)运行的解决方案,在ANSYS LS-DYNA中将应力初始化为小应变的规定几何形状。 显式解决方案基于drelax文件中包含的隐式X,Y,Z位移和旋转(使用REXPORT命令创建)。】【1,先读入隐士位移,2,将位移通过动力松弛转化为初始应力。】
! Increase the pressure load after a bit to introduce plasticity in
! the beam. The beam should remain bent in the XZ plane (due to the
! thermal load) while bending further downward in the YZ plane.
*dim,etime,,5,1,1 !数组
*dim,epress,,5,1,1
etime(1)=0.0,0.025,0.050,0.100,0.201 ! extend curve out
epress(1)=1.1e5,1.1e5,2.2e5,2.2e5,4.4e5 ! force into plasticity
edload,add,press,4,ebeamtop,etime,epress ! pressure (N/m^2) on beam top
dlist,all,all ! keep beam restraints from previous implicit run保持隐士分析的约束
edrst,100
edhtime,200
edhist,nbeamtop !指定组元的时间历程输出
edhist,ebeamtop
edenergy,1,1,1,1
edout,glstat
edopt,add,,both !结果文件类型ansys及lsdyna
edwrite,both,,k !K文件类型及写K文件
nsel,all
esel,all
save
solve
fini
/post1
set,first
/dscale,,10 ! exaggerate displacement
/title, ANSYS/LS-DYNA Dynamic Relaxation Analysis
plnsol,s,eqv,2
/wait,5
set,last
/title, ANSYS/LS-DYNA Transient Dynamic Analysis (Plastic State)
plnsol,s,eqv,2
/wait,5
save
!!! fini
!!! /exit,nosav