案例：LS-DYNA热固耦合（隐式-显式耦合）

步骤：

1）描述：

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。

需要选择ANSYS MULTIPHYSICS   ls-dyna模块

1）preload.inp包含的内容解读：

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 An alysis

/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 an alysis

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

fini

! = = = = = = = = = = = = = 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 A nalysis

/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 

!        an alysis, since implicit-to-explicit sequential solutions 

!        assume linear elastic material properties and s mall 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 a nalysis

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 an alysis

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 An alyses

/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 material data tables

fini

/solu

time,0.2               ! termination time (seconds)

rexport,dyna,,,,,preload,rst   ! create drelax file， Exports displacements from an implicit run to ANSYS LS-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>An alysis 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 An alysis

plnsol,s,eqv,2

/wait,5

set,last

/title, ANSYS/LS-DYNA Transient Dynamic An alysis (Plastic State)

plnsol,s,eqv,2

/wait,5

save

!!! fini

!!! /exit,nosav