搜索
55..11二次衬砌结构力学分析/TITLE，Mechanicalanalysisonrailwaytunnel2ndlining!确定分析标题/NOPR!菜单过滤设置/PMETH，OFF，0KEYW，PR_SET，1KEYW，PR_STRUC，1!保留结构分析部分菜单/COM，/COM，PreferencesforGUIfilteringhavebeensettodisplay:/COM，Structural!/PREP7!进入前处理器ET，1，BEAM3!设置梁单元类型ET，2，COMBIN14!设置弹簧单元类型R，1，0.4，0.0053333，0.4，，，，!设置梁单元几何常数R，2，400e6，，，!设置弹簧单元几何常数MPTEMP，，，，，，，，!设置材料模型MPTEMP，1，0MPDATA，EX，1，，30.0e9!输入弹性模量MPDATA，PRXY，1，，0.2!输入泊松比MPTEMP，，，，，，，，!设置材料模型MPTEMP，1，0MPDATA，DENS，1，，2500!输入密度SAVE!保存数据库1．建立几何模型K,1,,,,!创建关键点（隧道二次衬砌）K,2,4.71,-1.82,,K,3,-4.71,-1.82,,K,4,0,-3.75,,K,5,0,5.05,,K,20,5.6,-2.162,,!创建关键点（地层弹簧）K,30,-5.6,-2.16,,K,40,0,-4.75,,K,50,0,6,,!创建隧道衬砌线LARC,2,5,1,5.05,!创建圆弧线（拱顶部）LARC,5,3,1,5.05,LARC,2,3,4!创建圆弧线（仰拱部）第1章大型有限元软件ANSYS简介2!创建地层弹簧线LARC,20,50,1,6,!创建圆弧线（拱顶部）LARC,50,30,1,6,LARC,20,30,40!创建圆弧线（仰拱部）SAVE!保存数据2．单元网格划分设置单元大小并将所有直线划分单元，其单元图如图5-8所示。LESIZE,ALL,,,10,,1,,,1,!设置单元大小,每条弧线划分成10个单元TYPE,1!设置将要创建单元的类型MAT,1!设置将要创建单元的材料REAL,1!设置将要创建单元的几何常数LMESH,1,6,1!将所有直线划分单元/PNUM,KP,0!以下为显示单元编号和颜色/PNUM,ELEM,1/REPLOT!重新显示SAVETYPE,2!设置将要创建单元的类型MAT,1!设置将要创建单元的材料REAL,2!设置将要创建单元的几何常数E,1,31!通过两个节点创建弹簧单元E,2,32E,3,33E,4,34E,5,35E,6,36E,7,37E,8,38E,9,39E,10,40E,11,41E,12,42E,13,43E,14,44E,15,45E,16,46E,17,47E,18,48E,19,49E,20,50E,21,51E,22,52E,23,53E,24,54E,25,55第1章大型有限元软件ANSYS简介3E,26,56E,27,57E,28,58E,29,59E,30,60Lclear,4,6,1!清除用于创建地层弹簧单元的外层梁单元LDELE,4,6,1,1!删除外层直线Finish!返回MainMenu主菜单5.1.2加载与求解/SOL!进入求解器d,31,ux,0,0,60,1,uy,!在“Ux”和“Uy”两个方向的施加约束ACEL,0,10,0,!在Y方向施加重力加速度F,2,Fx,0!在节点上施加X方向集中力F,13,Fx,43554.43356F,14,Fx,86574.64508F,15,Fx,128464.6048F,16,Fx,168285.8813F,17,Fx,204799.5937F,18,Fx,236448.4444F,19,Fx,261396.9365F,20,Fx,277795.0781F,21,Fx,283894.0611F,12,Fx,247397.3915F,30,Fx,190308.0663F,29,Fx,149683.6899F,28,Fx,103226.8339F,27,Fx,52665.0399F,26,Fx,0F,25,Fx,-52665.0399F,24,Fx,-103226.8339F,23,Fx,-149683.6899F,22,Fx,-190308.0663F,1,Fx,-247397.3915F,3,Fx,-283894.0611F,4,Fx,-277795.0781F,5,Fx,-261396.9365F,6,Fx,-236448.4444F,7,Fx,-204799.5937F,8,Fx,-168285.8813F,9,Fx,-128464.6048F,10,Fx,-86574.64508F,11,Fx,-43554.43356F,2,Fy,-449636.88!在节点上施加Y方向集中力第1章大型有限元软件ANSYS简介4F,13,Fy,-441210F,14,Fy,-416229.66F,15,Fy,-375629.1F,16,Fy,-320951.4F,17,Fy,-254238.6F,18,Fy,-178008.6F,19,Fy,-95102.7F,20,Fy,0F,21,Fy,82772.64F,12,Fy,259324.92F,30,Fy,413398.46F,29,Fy,454320.04F,28,Fy,484308F,27,Fy,502604.08F,26,Fy,508719.08F,25,Fy,502604.08F,24,Fy,484308F,23,Fy,454320.04F,22,Fy,413398.46F,1,Fy,259324.92F,3,Fy,82772.64F,4,Fy,0F,5,Fy,-95102.7F,6,Fy,-178008.6F,7,Fy,-254238.6F,8,Fy,-320951.4F,9,Fy,-375629.1F,10,Fy,-416229.66F,11,Fy,-441210SaveNROPT,FULL,,!采用全牛顿－拉普森法进行求解Allsel!选择所有内容Outres,all,all!输出所有内容Solve!求解计算Finish!求解结束返回MainMenu主菜单SAVE5.1.3后处理1．初次查看内力和变形结果/POST1!进入后处理器PLDISP,1!绘制变形和未变形图ETABLE,,SMISC,6!6、12表示弯矩ETABLE,,SMISC,12ETABLE,,SMISC,1!1、7表示轴力第1章大型有限元软件ANSYS简介5ETABLE,,SMISC,7ETABLE,,SMISC,2!2、8表示剪力ETABLE,,SMISC,8查看内力,包括弯矩、轴力和剪力，如图5-12、图5-13和图5-14所示。路径：GeneralPostprocPlotResultsContourPlotLineElemRes。PLLS,SMIS6,SMIS12,-1,0!绘制弯矩图ESEL,R,TYPE,,1!仅显示单元类型1PLLS,SMIS1,SMIS7,1,0!绘制轴力图PLLS,SMIS2,SMIS8,1,0!绘制剪力图2．去除受拉弹簧再计算Finish!结束后处理器操作/sol!进入求解器Ekill,62!杀死62号地层弹簧单元Ekill,71Ekill,70Ekill,73Ekill,74Ekill,88Ekill,86Ekill,87Ekill,85Ekill,86SAVEAllsel!选择所有内容Solve!求解计算Finish!求解结束返回MainMenu主菜单SAVE3．查看最后计算结果/POST1ETABLE,REFL!更新单元表数据PRETAB,SMIS6,SMIS12,SMIS1,SMIS7,SMIS2,SMIS8!打印单元表数据PRNSOL,DOF,!打印节点位移第1章大型有限元软件ANSYS简介655..22台阶法施工过程仿真分析1．材料、实常数和单元类型定义/TITLE，Mechanicalanalysisonrailwaytunnel1ndlining!确定分析标题/NOPR!菜单过滤设置/PMETH，OFF，0KEYW，PR_SET，1KEYW，PR_STRUC，1!保留结构分析部分菜单/COM，PreferencesforGUIfilteringhavebeensettodisplay:/COM，Structural/PREP7!进入前处理器ET,1,PLANE42!设置实体单元类型KEYOPT,1,1,0KEYOPT,1,2,0KEYOPT,1,3,2!设置为平面应变模式KEYOPT,1,5,0KEYOPT,1,6,0ET，2，BEAM3!设置梁单元类型ET,3,LINK1!设置杆单元类型R,1,0.2,0.0008,0.2,,,,!设置梁单元几何常数R,2,0.0005,,!设置杆单元几何常数MPTEMP,,,,,,,,MPTEMP,1,0MPDATA,EX,1,,3.2e9!输入弹性模量（围岩）MPDATA,PRXY,1,,0.32!输入泊松比（围岩）MPDATA,DENS,1,,2200!输入密度（围岩）MPDATA,EX,2,,27.5e9!输入弹性模量（喷射混凝土）MPDATA,PRXY,2,,0.2!输入泊松比（喷射混凝土）MPDATA,DENS,2,,2500!输入密度（喷射混凝土）MPDATA,EX,3,,200e9!输入弹性模量（锚杆）MPDATA,PRXY,3,,0.3!输入泊松比（锚杆）MPDATA,DENS,3,,7800!输入密度（锚杆）SAVE!保存数据库2．建立几何模型K,1,0,0,,!创建隧道轮廓线关键点K,2,5.45,0,,K,3,0,5.45,,K,4,-5.45,0,,K,5,-5.0838,-1.964,,K,6,0,-4.15,,第1章大型有限元软件ANSYS简介7K,7,5.0838,-1.964,,K,8,8.45,0,,!创建锚杆加固区域关键点K,9,0,8.45,,K,10,-8.45,0,,K,11,13,0,,K,12,0,13,,K,13,-13,0,,K,14,-13,13,,K,15,13,13,,K,16,8.45,-8.45,,K,17,-8.45,-8.45,,K,18,-13,-13,,K,19,13,-13,,K,20,0,26,,!创建计算区域关键点K,21,13,26,,K,22,-13,26,,K,23,-13,-34,,K,24,13,-34,,K,25,0,-34,,K,26,50,-34,,K,27,-50,-34,,K,28,-50,26,,K,29,50,26,,K,30,50,13,,K,31,50,0,,K,32,50,-13,,K,33,-50,-13,,K,34,-50,0,,K,35,-50,13,,K,36,0,-8.45K,37,0,-13K,38,2.8653,-3.5371K,39,-2.8653,-3.5371SAVELARC,2,3,1,5.45,!*画隧道轮廓线LARC,3,4,1,5.45,!*LARC,4,5,1,5.45,LARC,5,6,39!*LARC,7,2,1,5.45,LARC,8,9,1,8.45,!*画锚杆加固区域线LARC,9,10,1,8.45,LSTR,1,2!*画其它分割线LSTR,1,3LSTR,1,4LSTR,1,6LSTR,2,8第1章大型有限元软件ANSYS简介8LSTR,4,10LSTR,8,11LSTR,11,15LSTR,15,12LSTR,12,9LSTR,12,14LSTR,14,13LSTR,13,10LSTR,10,17LSTR,13,18LSTR,8,16LSTR,11,19LSTR,17,36LSTR,36,16LSTR,6,36LSTR,36,37LSTR,18,37LSTR,37,19LSTR,37,25LSTR,19,24LSTR,18,23L