yangchun8611 发表于 2007-4-23 15:50

ansys使用经验(转帖)个人觉得很有道理

使用Ansys软件建模的经验与技巧
1.始终注意保持使用一致的单位制;
2求解前运行allsel命令
求解前运行allsel命令。要不然,某些已经划分网格的实体而没有被选择,那么加在实体模型上加的荷载可能会没有传到nodes or elements上去;
3网格划分问题
牢记《建模与分网指南》上有关建模的忠告。网格划分影响模型是否可用,网格划分影响计算结果的可接受程度;
自适应网格划分(ADAPT)前必须查自适应网格划分可用单元,在ansys中能够自适应网格划分的单元是有限的。
网格划分完成后,必须检查网格质量!权衡计算时间和计算精度的可接受程度,必要时应该refine网格
4 实体建模布尔运算
应用实体建模以及布尔运算(加、减、贴、交)的优势解决建立复杂模型时的困难;但是,没有把握时布尔运算将难以保证成功!
5 计算结果的可信度
一般来说,复杂有限元计算必须通过多人,多次,多种通用有限元软件计算核对,互相检验,相互一致时才有比较可靠的计算结果。协同工作时必须对自己输入数据高度负责,并且小组成员之间保持良好的沟通;有限元分析不是搞什么“英雄主义”,而需要多方面的质量保证措施。
6了解最终所需要的成果
建立模型之前,应该充分了解最终要求提交什么样式的成果,这样能形成良好的网格,早期良好的建模规划对于后期成果整理有很大的帮助;
7 撰写分析文档
文档与分析过程力求保持同步,有利于小组成员之间的沟通和模型的检验和查证;
8 熟悉命令
对没有把握的命令应该先用简单模型熟悉之,千万不能抱有“撞大运”的想法;
9 多种单元共节点
不同单元使用共同节点时注意不同单元节点自由度匹配问题导致计算结果的正确与否(《建模与分网指南》P 8 )
三维梁单元和壳单元的节点自由度数一致,但是应该注意到三维梁单元的转动自由度和 壳单元的转动自由度的含义不一样。壳的ROTZ不是真实的自由度,它与平面内旋转刚度相联系,在局部坐标中壳的单元刚度矩阵ROTZ对应的项为零,对此不能将梁与壳单元仅仅有一个节点相连,例外的是当shell43 or shell63(两者都有keyopt(3)=2)的Allman旋转刚度被激活时。
Solid65 单元和 shell63 单元相连,相应平动自由度的节点力会传到实体块单元上,但是shell63单元的转动自由度的节点唯一则不会传到相连的 solid65单元上。
10 查找文献资料确定混凝土的材料参数输入( Tb, concr, , , )
11 预测内存和磁盘空间
大型复杂模型(例如10万个节点,非线性问题,多工况问题,1000步以上的瞬态分析等等)求解之前预测求解所需要的求解时间、内存和磁盘空间,使分析尽在掌握之中;
12 收敛问题
影响收敛(不收敛,或者收敛缓慢)的原因很多,《非线性分析指南》一书上有很多关于避免发生收敛问题的建议;
对于以下参数,可以试一试这些参数对收敛速度以及结果精度的影响
neqit = 6~25?
加载荷载步大小 = ?
接触单元的实常数 = ? 例如接触刚度的大小取值必须权衡计算结果精度(穿透大小)和收敛问题( 收敛时间 )两者的可接受程度,需要经验值或者试算;
13 启动重分析

14 两个相贯的薄壁圆筒建模,壳单元没有公共节点
Element Connectivity Error, 8-Node Curved Shell Elements
In this image, the red stiffener was intended to be welded to the purple pipe. Note that the elements of the red stiffener do not match up with those on the pipe. There is no connection, and the meshing was done independently. This is due to a geometric modeling error by the user (me). There are superimposed curved lines where the interface is located. There should have been a shared line for the connection to have worked. I found this only because of careful examination of the model -- I had already run a stress analysis.
What to do about these error concerns? Read and think. Share and listen to ideas and concerns with others. Review your own work, and the work of your co-workers. (Recently an experienced co-worker who does not even do FEA work asked me if I had eliminated the added mass of water in pipes when evaluating shipping loads on a product. I hadn't. Eliminating the added mass got rid of a high-stress problem. These errors are very easy to make.) Be friendly. Communicate with other departments. Have a check list and design reviews. Never use FEA blindly, or believe the results of an analysis without some critical review. Accept a critical review without taking it personally. Develop a good understanding of the intent of the design codes that regulate your work. Consult an expert when it is appropriate. Pay attention to the ethics and standards of your professional association. Choose your employer wisely. (Some of these things you were supposed to have learned in Kindergarten, but life isn't always that simple.)
解决方法:通过volumn建模形成相贯线,该方法建模使面相交处共线,xmesh后有公共nodes
15 选择集的应用
为了利用选择集cm / xsel的强大功能,可以合理定义线,面的实常数real属性,为了选择操作方便而赋予更多的单元实常数号,材料号

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








页: [1]
查看完整版本: ansys使用经验(转帖)个人觉得很有道理