发布时间 : 星期三 文章ansys中LS-DYNA 2D金属切削模拟步骤更新完毕开始阅读bd39e467b84ae45c3b358c33
在ANSYS Launcher界面中,选择ANSYS Mechanical/LS-DYNA
1、菜单过滤
Main Menu→Preprocessor→LD-DYNA Explicit→OK
2、设置文件名及分析标题
Utility Menu→File→change Jobname→2D cutting→New log and error file :YES→OK Utility Menu→File→change Title→cutting analysis →OK 3、选择单元类型
Main menu→preprocessor→Element Type→Add/Edit/Delete→Add→2D solid 162→OK→options→选择const.stress ;Lagrangian→OK 4、定义材料模型 (1) 定义刀具材料模型
Main menu→preprocessor→Material Props→Material Models→rigid material→ 输入:DENS:5.2e3 ;EX:4.1e11 ;NUXY:0.3 ;选择“Y and Zdisps” ;“All rotations”→OK
(2) 定义工件Johnson-cook材料模型
Main menu→preprocessor→Material Props→Material Models→Gruneisen→Johnson-cook→输入:DENS:7.8e3 ;EX:2.06e11 ;NUXY:0.3
A:507;B:320;C:0.28;n;0.064;m=1.06
D1:0.15;D2:0.72;D3:1.66;D4:0.005;D5:--0.84
5、创建几何模型
(1)创建工件模型
Main menu→preprocessor→Create→Areas→Rectangle→By Dimensions→输入:X1,X2:0,5;Y1,Y2:0,3→OK
(2)创建刀片模型
Main menu→preprocessor→Create→Keypionts→In Active CS→依次输入:
keypoint number:5,X、Y、Z :5.1,2.9,0; keypoint number:6,X、Y、Z :6,3.228,0; keypoint number:7,X、Y、Z :6,4,0; keypoint number:8,X、Y、Z :5.294,4,0→OK
6、网格划分
(一)
(1) 对刀片进行网格划分
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取刀片边线→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:10→OK
(2) 对刀尖半圆进行网格划分
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取刀尖半圆→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:3→OK
(3) 确定刀片的单元属性
Main menu→preprocessor→Meshing→Mesh Attributes→Picked Aeras→选取刀片→Apply→确定材料号和单元类型号为1→OK
(4) 刀片网格划分
Main menu→preprocessor→Meshing→MeshTool→Mesh:Aeras;shape:Tri;free→Mesh→选取刀片→OK
(二)
(5) 对工件进行网格划分
切分工件
Utility menu →Workplane→Wp settings→Grid and Triad→Minimum ,maximum:-5,5 ;
Spacing:1.0→OK
平移和旋转工作平面并用其切分工件
Utility menu →Workplane→Offset wp by incremens→X,Y,Z offsets:0,2.5,0;XY,YZ,ZX angle:0,90,0→OK
Main menu→preprocessor→Modeling→operate→Booleans→Divide→Areas by wkplane→选取工件→OK
取消工作平面显示
Utility menu→workplane→Display workingplane→ 等分接触区域相关Y向线段
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取工件接触区Y向线段(两条)→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:10→OK
等分接触区域相关X向线段
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取工件接触区X向线段(两条)→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:40→OK
等分接触区域不相关Y向线段
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取工件接触区Y向线段(两条)→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:25→OK
等分接触区域不相关X向线段
Utility Menu→Select→Entities→Lines :By Num/Pick→Apply→选取工件接触区X向线段(底边)→OK
Main menu→preprocessor→Meshing→Size contrls→Manualsize→Lines→All lines→NDIV:30→OK
确定工件的单元属性
Main menu→preprocessor→Meshing→Mesh Attributes→Picked Aeras→选取工件→Apply→确定材料号为2和单元类型号为1→OK
工件网格划分
Main menu→preprocessor→Meshing→MeshTool→Mesh:Aeras;shape:Quad;mapped→Mesh→选取工件→OK 7、建立part
Main menu→preprocessor→LS-DYNA options→part options→create all part→OK
(part1:刀具;part2:工件) Plot→parts(不同颜色显示单元) 8、定义接触信息
Main menu→preprocessor→LS-DYNA options→contact→Define contact→surface to surf;Eroding;静、动摩擦系数为0.15、0.10→OK→弹出contact options对话框,确定接触件(工件),目标件(刀片)→OK 9、施加边界条件
Utility menu→select→Entities→Nodes :By Location :X Coordinates→Min,Max:-0.01,0.01;From Full→Apply(选中左侧边所有节点)
Main menu→preprocessor→LS-DYNA options→Constraints→Apply→on nodes→pick All→All DOF→OK