3楼
18 UPGEOM 和 MPCHG 的应用
! UPGEOM更新几何形状
!a.rst为计算结果文件名,最后一个为目录
!这两个参数应根据你的计算情况定
UPGEOM,1,LAST,LAST,NEW,rst,F:\729\
! MPCHG弹性模量恢复为真值
esel,s,mat,,3
mpchg,4,all
• You might be tempted to try to deactivate or reactivate elements by changing their material properties [ MPCHG ] ( Main Menu>Preprocessor>Material Props>Change Mat Num ).
However, you must proceed cautiously if you attempt such a procedure. The safeguards and restrictions that affect "killed" elements will not apply to elements that have their material properties changed in SOLUTION. (Element forces will not be automatically zeroed out;nor will strains, mass, specific heat, etc.) Many problems could result from careless use of MPCHG . For instance, if you reduce an element’s stiffness to almost zero, but retain its mass, it could result in a singularity if subjected to acceleration or inertial effects.
One application of MPCHG would be in modeling construction sequences in which the strain history of a "born" element is maintained. Using MPCHG in such cases will enable you to capture the initial strain experienced by elements as they are fitted into the displaced nodal configuration.
19 Ansys 中的坐标系统,使用各种坐标系时应该明白在各处理器中输入输出会受到那些坐标系的影响
整体和局部坐标系CSYS---用于定位几何形状参数的空间位置
显示坐标系DSYS---用于几何形状参数的列表和显示
节点坐标系---定义节点自由度方向和节点结果数据的方法。输入数据时受到节点坐标系影响的有:约束自由度(方程),力,主(从)自由度;在/POST26中在节点坐标系下输出文件和显示的数据结果有:自由度解,节点荷载,反作用荷载;
Forces are defined in the nodal coordinate system. The positive directions of structural forces and moments are along and about the positive nodal axis directions. The node and the degree of freedom label corresponding to the force must be selected [ NSEL , DOFSEL ].
单元坐标系---每个单元都有自己的坐标系,单元坐标系用于确定材料特性主轴,加面压力和和单元结果数据(如应力和应变)的输出方向;ANSYS规定了单元坐标系的缺省方向;许多单元都有keyopts可用于修改单元坐标系的缺省方向;对于面和体单元而言,可以用ESYS命令将单元坐标系的方向调整到已定义的局部坐标系;
结果坐标系RSYS---用来列表、显示或者在/POST1中将节点和单元结果转换到特定的坐标系中。在/POST1中结果数据换算到结果坐标系(RSYS)下记录。定义路径时,可以用系列命令*GET, ACTSYS, ACTIVE,CSYS $ RSYS, ACTSYS使结果坐标系与激活的坐标系(用于定义路径)相匹配
求解坐标系---大多数模型叠加技术(PSD,CQC,SRSS)是在求解坐标系中进行的,使用RSYS,SOLU命令来避免在结果坐标系中发生变换,使结果数据保持在求解坐标系中。
20 Ansys 5.7通过函数定义边界条件
利用函数可以很简单方便地定义复杂边界条件和载荷(将边界条件当作函数处理(即方程))。该特性是5.6 中介绍的表格化边界条件的扩展功能。用户可以创建大量函数并存储起来,以便于将来使用。
5.6的表格化边界条件(Tabular boundary conditions)
Tabular boundary conditions ( VALUE = % tabname %) are available only for structural (UX, UY, UZ, ROTX, ROTY, ROTZ) and temperature degree of freedom (TEMP) labels and are valid only in static ( ANTYPE ,STATIC) and full transient ( ANTYPE ,TRANS) analyses.
滞回曲线——位移加载
*DIM,dis,TABLE,9,1,,TIME, ,
DIS(1,0) = 0,1,2,3,4,5,6,7,8
DIS(1,1) = 0,3,0,-3,0,4,0,-4,0
D,22, , %DIS% , , , ,UZ, , , , ,
ansys 5.6 help files------- 2.6.3. Applying Loads Using TABLE Type Array Parameters
优点:
 将复杂载荷和边界条件定义成基本变量和因变量的连续或非连续方程。
 提供创建和运用函数的极易操作的GUI 界面。
应用 :
 该特性适用于所有ANSYS家族产品。
 该特性适用于ANSYS程序的所有过程,支持TIME, TEMP, X, Y, Z, VELOCITY和PRESSURE等基本变量。
21 automatic time stepping
For nonlinear problems, automatic time stepping determines the amount of load increment between substeps,
回复