ANSYS热结构耦合分析实例.docx
《ANSYS热结构耦合分析实例.docx》由会员分享，可在线阅读，更多相关《ANSYS热结构耦合分析实例.docx（16页珍藏版）》请在冰豆网上搜索。
ANSYS热结构耦合分析实例
ANSYS热-结构耦合分析实例
（1）
/PREP7
/TITLE,Part1:
heattransferanalysis
ET,1,SOLID70!
定义单元类型
!
-----------------------------------------------------------------
!
设置参数
!
单位制为：
力-N;长度-m;温度-；时间-s；
!
-----------------------------------------------------------------
W_col=0.2039!
柱截面宽度
H_col=0.2062!
柱截面高度
tf_col=0.0125!
柱翼缘厚度
tw_col=0.0083!
柱腹板厚度
B_col=（W_col-tw_col）/2!
柱翼缘伸出长度
D_col=H_col-2*tf_col!
柱腹板净高
W_beam=0.165!
梁截面宽度
H_beam=0.3038!
梁截面高度
tf_beam=0.0102!
梁翼缘厚度
tw_beam=0.0061!
梁腹板厚度
B_beam=（W_beam-tw_beam）/2!
梁翼缘伸出长度
D_beam=H_beam-2*tf_beam!
梁腹板净高
Dis_hor=5.5!
框架水平跨间距
Dis_ver=3.0!
框架竖向层高
pp=（W_col-W_beam）/2
!
------------------------------------------------------------------------
!
定义热分析材料特性,包括导热性，比热，密度等
!
------------------------------------------------------------------------
MPTEMP,,20,800,900,1000!
定义随温度变化的钢材的导热性
MPDATA,KXX,1,,53.334,27.36,27.36,27.36
MPTEMP!
清除当前温度场
MPTEMP,,20,100,180,260,380!
定义随温度变化的钢材的比热
MPDATA,C,1,,439.8,487.62,522.33,550.75,596.52
MPTEMP,,500,600,640,720,735
MPDATA,C,1,,666.5,759.92,798.67,1388,5000
MPTEMP,,750,830,900,1000
MPDATA,C,1,,1483,725,650,650
MP,DENS,1,7850!
定义钢材的密度
!
------------------------------------------------------------------------
!
建立分析模型
!
------------------------------------------------------------------------
!
生成第一根柱：
N,1,-H_col/2,,-W_col/2!
产生构成柱截面的节点
N,2,-H_col/2,,-W_col/2+pp
NGEN,4,1,2,,,,,（B_col-pp）/3
N,6,-H_col/2,,tw_col/2
NGEN,4,1,6,,,,,（B_col-pp）/3
N,10,-H_col/2,,W_col/2
NGEN,2,10,1,10,1,tf_col
NGEN,10,6,15,16,1,D_col/10
NGEN,2,60,11,20,1,D_col
NGEN,2,10,71,80,1,tf_col
NGEN,2,100,all,,,,（Dis_ver-H_beam/2）/60!
将已生成的节点沿y方向偏移（Dis_ver-H_beam/2）/60拷贝一层，节点号加100
!
从已产生的两层节点生成第一层单元
E,1,2,12,11,101,102,112,111!
定义翼缘上第一个单元
EGEN,9,1,1!
沿翼缘长度拷贝9个单元
E,15,16,22,21,115,116,122,121!
定义腹板上第一个单元，编号为10
EGEN,10,6,10!
拷贝单元10形成腹板
E,71,72,82,81,171,172,182,181!
定义另一翼缘上一个单元，编号20
EGEN,9,1,20!
拷贝单元20形成另一翼缘
!
将第一层单元沿y方向拷贝60层，ANSYS自动生成所有的节点。
节点编号每层加100。
EGEN,60,100,1,28,1,,,,,,0,（Dis_ver-H_beam/2）/60
!
将柱的模型继续向上延伸梁的截面高度，生成梁柱节点。
!
节点处单元尺寸尽量与梁的截面单元尺寸一致。
NSEL,S,NODE,,6001,6090,1!
将顶层节点向上偏移梁的翼缘厚度，
NGEN,2,100,ALL,,,,tf_beam!
并生成一层单元
EGEN,2,100,1653,1680,1
NSEL,ALL
!
NSEL,S,NODE,,6101,6190!
将顶层节点向上偏移梁的腹板净高度，
NGEN,11,100,ALL,,,,D_beam/10!
并生成10层单元
EGEN,11,100,1681,1708,1
NSEL,ALL
!
NSEL,S,NODE,,7101,7190!
将顶层节点向上偏移梁的翼缘厚度
NGEN,2,100,ALL,,,,tf_beam!
并生成一层单元
EGEN,2,100,1961,1988,1
NSEL,ALL
!
将实体模型的柱向上延伸H_beam的高度，避免梁单元和实体单元在梁柱节点处切换
NSEL,S,NODE,,7201,7290!
生成6层单元，每层高H_beam/6
NGEN,7,100,ALL,,,,H_beam/6
EGEN,7,100,1989,2016,1
NSEL,ALL
!
第一根实体模型柱完成。
!
共计：
节点79层，每层编号1-90，逐层加100，顶层编号7801-7890
!
单元78层，自动编号。
每层28个，共28*78=2184个
!
!
拷贝第一根柱生成第二根柱
NGEN,2,10000,ALL,,,Dis_hor!
拷贝所有的节点，节点号加10000
EGEN,2,10000,1,2184,1!
拷贝所有的单元
!
!
生成梁
!
梁被夹在两根柱之间，实际长度为Dis_hor-H_col
!
生成左侧形成一个梁截面的所有节点，梁的节点编号从20001开始
N,20001,H_col/2,Dis_ver-H_beam/2,-W_beam/2
NGEN,4,1,20001,,,,,B_beam/3
N,20005,H_col/2,Dis_ver-H_beam/2,tw_beam/2
NGEN,4,1,20005,,,,,B_beam/3
NGEN,2,10,20001,20008,1,,tf_beam
NGEN,10,6,20014,20015,1,,D_beam/10
NGEN,2,60,20011,20018,1,,D_beam
NGEN,2,10,20071,20078,1,,tf_beam
!
沿x方向偏移（Dis_hor-H_col）/100拷贝一层节点，节点编号加100
NGEN,2,100,20001,20090,,（Dis_hor-H_col）/100
!
生成梁的第一层截面单元
!
两根柱单元总数为4368，故梁的单元编号从4369开始。
E,20001,20002,20012,20011,20101,20102,20112,20111!
定义单元4369
EGEN,7,1,4369!
拷贝单元4369形成一个翼缘
E,20014,20015,20021,20020,20114,20115,20121,20120!
定义单元4376
EGEN,10,6,4376!
拷贝单元4376形成腹板
E,20071,20072,20082,20081,20171,20172,20182,20181!
定义单元4386
EGEN,7,1,4386!
拷贝单元4386形成另一翼缘
!
沿x方向拷贝100层生成整根梁，每层高度（Dis_hor-H_col）/100
EGEN,100,100,4369,4392,1,,,,,,（Dis_hor-H_col）/100
!
梁的实体模型完成
!
总计：
梁的节点为101层，每层编号1-88。
从20001开始，逐层加100
!
左端截面的节点为20001-20088；右端截面的节点为30001-30088
!
每层单元数为24个，总计24*100=2400个。
单元编号为4369-6768
!
----------------------------------------------------------------------
!
建立梁和柱连接处的耦合关系。
!
----------------------------------------------------------------------
CPINTF,all,0.002
FINISH
!
/SOLU
ANTYPE,TRANS!
定义分析类型
TUNIF,20!
定义初始温度
!
-----------------------------------------------------------------------
!
定义边界条件，并求解
!
-----------------------------------------------------------------------
!
选择梁的上翼缘上表面，定义为HTUP
NSEL,S,NODE,,20081,30081,100
NSEL,A,NODE,,20082,30082,100
NSEL,A,NODE,,20083,30083,100
NSEL,A,NODE,,20084,30084,100
NSEL,A,NODE,,20085,30085,100
NSEL,A,NODE,,20086,30086,100
NSEL,A,NODE,,20087,30087,100CM,HTUP,NODE!
定义以上所选节点为HTUP
NSEL,ALL
!
选择梁的下翼缘下表面，定义为HTDOWN
NSEL,S,NODE,,20001,30001,100
NSEL,A,NODE,,20002,30002,100
NSEL,A,NODE,,20003,30003,100
NSEL,A,NODE,,20004,30004,100
NSEL,A,NODE,,20005,30005,100
NSEL,A,NODE,,20006,30006,100
NSEL,A,NODE,,20007,30007,100
CM,HTDOWN,NODE!
定义以上所选节点为HTDOWN
NSEL,ALL
!
选择梁的左侧，定义为HTLEFT
NSEL,S,NODE,,20011,30011,100
NSEL,A,NODE,,20012,30012,100
NSEL,A,NODE,,20013,30013,100
NSEL,A,NODE,,20014,30014,100
NSEL,A,NODE,,20020,30020,100
NSEL,A,NODE,,20026,30026,100
NSEL,A,NODE,,20032,30032,100
NSEL,A,NODE,,20038,30038,100
NSEL,A,NODE,,20044,30044,100
NSEL,A,NODE,,20050,30050,100
NSEL,A,NODE,,20056,30056,100
NSEL,A,NODE,,20062,30062,100
NSEL,A,NODE,,20068,30068,100
NSEL,A,NODE,,20074,30074,100
NSEL,A,NODE,,20071,30071,100
NSEL,A,NODE,,20072,30072,100
NSEL,A,NODE,,20073,30073,100
CM,HTLEFT,NODE!
定义以上所选节点为HTLEFT
NSEL,ALL
!
选择梁的右侧，定义为HTRIGHT
NSEL,S,NODE,,20015,30015,100
NSEL,A,NODE,,20016,30016,100
NSEL,A,NODE,,20017,30017,100
NSEL,A,NODE,,20018,30018,100
NSEL,A,NODE,,20021,30021,100
NSEL,A,NODE,,20027,30027,100
NSEL,A,NODE,,20033,30033,100
NSEL,A,NODE,,20039,30039,100
NSEL,A,NODE,,20045,30045,100
NSEL,A,NODE,,20051,30051,100
NSEL,A,NODE,,20057,30057,100
NSEL,A,NODE,,20063,30063,100
NSEL,A,NODE,,20069,30069,100
NSEL,A,NODE,,20075,30075,100
NSEL,A,NODE,,20076,30076,100
NSEL,A,NODE,,20077,30077,100
NSEL,A,NODE,,20078,30078,100
CM,HTRIGHT,NODE!
定义以上所选节点为HTRIGHT
NSEL,ALL
!
施加热边界条件并求解
*DO,tm,60,180,60!
定义时间参数tm从60到600（秒）
Time,tm!
当前时间为tm
DELTIM,20!
定义初始时间步长
AUTOTS,ON!
打开自动步长控制
Temp=20+345*LOG10（8*tm/60+1!
计算环境空气温度
SF,HTUP,CONV,25,Temp!
对受热边界施加对流作用
SF,HTDOWN,CONV,25,Temp
SF,HTLEFT,CONV,25,Temp
SF,HTRIGHT,CONV,25,Temp
SF,HTUP,RDSF,0.7,1!
定义热辐射场
SF,HTDOWN,RDSF,0.7,2
SF,HTLEFT,RDSF,0.7,3
SF,HTRIGHT,RDSF,0.7,4
STEF,5.6696E-8!
定义Stefan-Boltzmann常数
TOFFST,273!
定义绝对温度偏差
SPCTEMP,1,Temp!
定义热辐射场的温度为火的温度
SPCTEMP,2,Temp
SPCTEMP,3,Temp
SPCTEMP,4,Temp
SOLVE
*ENDDO
FINISH
!
ANSYS热-结构耦合分析实例
（2）
结构分析
!
----------------------------------------------------------------------
!
/PREP7
/TITLE,Part2:
structuralanalysis
ET,1,SOLID45,1,1 !
对应于SOLID70的结构单元为SOLID45
ET,2,BEAM188 !
单元类型2为BEAM188
!
---------------------------------------------------------------
!
定义结构分析材料特性
!
---------------------------------------------------------------
fy=275E+6 !
常温下屈服应力
exx=2.1E+11 !
常温下杨氏模量
MPTEMP !
清除旧的温度场
MPTEMP,,20,100,200,300,400 !
定义随温度变化的杨氏模量
MPDATA,EX,1,,exx,exx,0.9*exx,0.8*exx,0.7*exx
MPTEMP,,500,600,700,800,900
MPDATA,EX,1,,0.6*exx,0.31*exx,0.13*exx,0.09*exx,0.0675*exx
MP,NUXY,1,0.3 !
定义泊松比
MP,ALPX,1,1.4E-5 !
定义热膨胀系数
!
定义随温度变化的应力-应变关系
TB,MISO,1,10,3 !
共10个温度，每个温度时的应力-应变由3个点描述
TBTEMP,20 !
20度时的应力-应变关系
TBPT,,fy/exx,fy
TBPT,,0.02,fy
TBPT,,0.15,fy
TBTEMP,100 !
100度时的应力-应变关系
TBPT,,fy/exx,fy
TBPT,,0.02,fy
TBPT,,0.15,fy
TBTEMP,200 !
200度时的应力-应变关系
TBPT,,0.807*fy/（0.9*exx）,0.807*fy
TBPT,,0.02,fy
TBPT,,0.15,fy
TBTEMP,300 !
300度时的应力-应变关系
TBPT,,0.613*fy/（0.8*exx）,0.613*fy
TBPT,,0.02,fy
TBPT,,0.15,fy
TBTEMP,400 !
400度时的应力-应变关系
TBPT,,0.420*fy/（0.7*exx）,0.420*fy
TBPT,,0.02,fy
TBPT,,0.15,fy
TBTEMP,500 !
500度时的应力-应变关系
TBPT,,0.360*fy/（0.6*exx）,0.360*fy
TBPT,,0.02,0.780*fy
TBPT,,0.15,0.780*fy
TBTEMP,600 !
600度时的应力-应变关系
TBPT,,0.180*fy/（0.310*exx）,0.180*fy
TBPT,,0.02,0.470*fy
TBPT,,0.15,0.470*fy
TBTEMP,700 !
700度时的应力-应变关系
TBPT,,0.075*fy/（0.130*exx）,0.075*fy
TBPT,,0.02,0.230*fy
TBPT,,0.15,0.230*fy
TBTEMP,800 !
800度时的应力-应变关系
TBPT,,0.050*fy/（0.090*exx）,0.050*fy
TBPT,,0.02,0.110*fy
TBPT,,0.15,0.110*fy
TBTEMP,900 !
900度时的应力-应变关系
TBPT,,0.0375*fy/（0.0675*exx）,0.0375*fy
TBPT,,0.02,0.060*fy
TBPT,,0.15,0.060*fy
!
-------------------------------------------------------------------
!
定义梁和柱的截面特性
!
-------------------------------------------------------------------
SECTYPE,1,beam,I,column !
定义柱截面为截面类型1
SECDATA,W_col,W_col,H_col,tf_col,tf_col,tw_col !
定义柱的截面尺寸
SECTYPE,2,beam,I,beam !
定义梁截面为截面类型2
SECDATA,W_beam,W_beam,H_beam,tf_beam,tf_beam,tw_beam !
定义梁截面尺寸
!
-----------------------------------------------------------------
!
用梁单元建立框架的剩余部分的模型
!
----------------------------------------------------------------
K,1,,Dis_ver+H_beam*1.5 !
定义生成框架的关键点
K,2,,2*Dis_ver
K,3,,3*Dis_ver
K,4,Dis_hor,Dis_ver+H_beam*1.5
K,5,Dis_hor,2*Dis_ver
K,6,Dis_hor,3*Dis_ver
K,7,Dis_hor+H_col/2,Dis_ver
K,8,2*Dis_hor
K,9,2*Dis_hor,Dis_ver
K,10,2*Dis_hor,2*Dis_ver
K,11,2*Dis_hor,3*Dis_ver
K,12,3*Dis_hor
K,13,3*Dis_hor,Dis_ver
K,14,3*Dis_hor,2*Dis_ver
K,15,3*Dis_hor,3*Dis_ver
K,100,-3,3 !
定义用于确定梁的主轴方向的关键点
K,200,5,20
!
生成线
L,1,2 !
线1-10用来生成柱单元
L,2,3
L,4,5
L,5,6
L,8,9
L,9,10
L,10,11
L,12,13
L,13,14
L,14,15
L,2,5 !
线11-18用来生成梁单元
L,3,6
L,7,9
L,5,10
L,6,11
L,9,13
L,10,14
L,14,15
!
定义线的属性
LSEL,S,LINE,,1,10,1 !
定义线1-10（柱）的属性
LATT,1,,2,,100,,1
LSEL,ALL
LSEL,S,LINE,,11,18,1 !
定义线11-18（梁）的属性
LATT,1,,2,,200,,2
LSEL,ALL
!
划分单元
LESIZE,ALL,0.3 !
定义单元尺寸
LMESH,ALL !
划分单元
!
------------------------------------------------------------------
!
建立耦合与约束关系
!
------------------------------------------------------------------
CPINTF,ALL,0.002 !
自动耦合实体模型部分
!
实体模型和线模型之间有三个接口：
两个柱端的连接，以及底层中跨的梁左端连接到第二根实体柱的侧面
!
建立关键点1和第一根柱柱端的连接
N1=NODE（0,Dis_ver+H_beam*1.5,0） !
找到对应于关键点1的节点号，标记为N1
num=0
升级会员 