Ansys使用经验ansys学习记录

1. Analysis Type： Any of seven analysis types offered in ANSYS: static, modal, harmonic, transient, spectrum, eigenvalue buckling, and substructuring. Whether the problem is linear or nonlinear will be identified here. 2. 在main menu上： The general postprocessor (POST1) is used to review results at one substep (time step) over the entire model. The time-history postprocessor (POST26) is used to review results at specific points in the model over all time steps. 3. ANSYS中的载荷可分为: 4. •自由度DOF - 定义节点的自由度（ DOF ） 值 (结构分析_位移、热分析_ 温度、电磁分析_磁势等) 5. •集中载荷 - 点载荷 (结构分析_力、热分析_ 热导率、电磁分析_ magnetic current segments) 6. •面载荷 - 作用在 表 关于同志近三年现实表现材料材料类招标技术评分表图表与交易pdf视力表打印pdf用图表说话 pdf 面的分布载荷 (结构分析_压力、热分析_热对流、电磁分析_magnetic Maxwell surfaces等) 7. •体积载荷 - 作用在体积或场域内 (热分析_ 体积膨胀、内生成热、电磁分析_ magnetic current density等) 8. •惯性载荷 - 结构质量或惯性引起的载荷 (重力、角速度等) 9. 压力数值为正表示其方向指向表面, 输入一个压力值即为 均布载荷,两个数值定义坡度压力 10. 加载时扩展的 （ inside ） 节点约束必须手工删除. 11. 在求解初始化前，应进行分析数据检查，包括下面内容: 1. •统一的单位 2. •单元类型和选项 3. •材料性质参数 1. –考虑惯性时应输入材料密度 2. –热应力分析时应输入材料的热膨胀系数 4. •实常数 (单元特性) 5. •单元实常数和材料类型的设置 6. •实体模型的质量特性 (Preprocessor > Operate > Calc Geom Items) 7. •模型中不应存在的缝隙 8. •壳单元的法向 9. •节点坐标系 10. •集中、体积载荷 11. •面力方向 12. •温度场的分布和范围 13. •热膨胀分析的参考温度 (与 ALPX 材料特性协调?) 12. 在求解过程中，应将OUTPUT窗口提到最前面。 ANSYS 求解过程中的一系列信息都将显示在此窗口中，主要信息包括: i. •模型的质量特性- 模型质量是精确的 - 质心和 质量矩的值有一定误差。 ii. •单元矩阵系数 - 当单元矩阵系数最大/最小值的比率 > 1.0E8 时将预示模型中的材料性质、实常数或几何模型可能存在问题。当比值过高时，求解可能中途退出。 iii. •模型尺寸和求解统计信息。 iv. •汇总文件和大小。 13. 没有获得结果的原因是什么? 往往是求解输入的模型不完整或存在错误，典型原因有: i. •约束不够! (通常出现的问题)。 ii. •当模型中有非线性单元 (如缝隙 gaps、滑块sliders、铰hinges、索cables等），整体或部分结构出现崩溃或“松脱”。 iii. •材料性质参数有负值, 如密度或瞬态热分析时的比热值。 iv. •未约束铰接结构，如两个水平运动的梁单元在竖直方向没有约束。 v. •屈曲 - 当应力刚化效应为负（压）时，在载荷作用下整个结构刚度弱化。如果刚度减小到零或更小时，求解存在奇异性，因为整个结构已发生屈曲。 14. •在任一方向，支反力总和必等于在此方向的载荷总和。 i. •节点反力列表: ii. •Main Menu: General Postprocessor > List Results > Reaction Solution... 15. •由于网格密度影响分析结果的精度，因此有必要验证网格的精度是否足够。 16. •有三种 方法 快递客服问题件处理详细方法山木方法pdf计算方法pdf华与华方法下载八字理论方法下载 进行网格精度检查： i. • 2. 观察（ Visual inspection ） 3. 误差估计 4. 将网格加密一倍，重新求解并比较两者结果。注意: 有些情况下这种做法不适用。 17. 误差估计只在进入后处理前PowerGraphics 被关闭的情况下进行。 (如果进入后处理后关闭 PowerGraphics则ANSYS将重新计算误差因子。) 18. “节点结果”（nodal solution）画出 19. 的是在节点处导出量的平均值，而“单元结果”（ element solution ）画出非平均量。 20. 泊松效应”（即，一个方向上的应力引起其它方向上的应变） 18. 只有到求解初始化时，才将模型中的载荷自动转化到有限元模型中的节点和单元上。 19. 误差估计只在进入后处理前PowerGraphics 被关闭的情况下进行。 (如果进入后处理后关闭 PowerGraphics则ANSYS将重新计算误差因子。) 20. •在给定节点处，可能存在不同的应力值。这是由以与此节点相连的不同单元计算而产生的。“节点结果”（nodal solution）画出的是在节点处导出量的平均值，而“单元结果”（ element solution ）画出非平均量。 21. •在弹性模量不同的材料交界处，应力分量会不连续。 (PowerGraphics 自动考虑到这一点并对此界面不进行平均处理。),在不同厚度的壳单元的交界处，大多数应力会不连续 。(PowerGraphics 自动考虑到这一点并对此界面不进行平均处理。), 在壳单元构成的尖角或连接处，某些应力分量不连续。 22. 在应力奇异处:.单元网格越是细化，越引起计算应力无限增加，并且不再收敛。 23. 打开智能网格并不影响映射网格的划分，映射网格仍然使用缺省尺寸。 24. 注意：在进行模态分析时，非线性特性如塑性和接触单元被忽略。模态分析得到的应力大小是任意的 21. 当你需要把几何模型的单位转换成另一套单位，比如说，从英寸到毫米，比例缩放就显得十分必要。Main Menu > Preprocessor > Operate > Scale > Volumes 22. 如果激励频率小于结构最低阶固有频率的1/3，则可以进行静力分析。在应力奇异点处网格越细化，应力值也随之增加且不收敛.当您选择了单元类型，您就选择并接受了相应单元类型的单元形函数。所以在您选择单元类型之前应查看单元形函数信息 25. After your solution runs for several minutes, Hit Ctrl-C, type SW2. and hit enter. LS-Dyna will print out the current time, energy values, and estimated run time remaining. The hourglass energy should be significantly lower than the total energy, if it's not, your solution may be diverging. 26. 当你确定你的收敛准则时记住以力为基础的收敛提供了收敛的绝对量度而以位移为基础的收敛仅提供了表观收敛的相对量度因此你应当如果需要总是使用以力为基础或以力矩为基础的收敛容限如果需要可以增加以位移为基础或以转动为基础的收敛检查但是通常不单独使用它们 27. 静态和瞬态处理的主要不同是在瞬态过 程分析中要激活时间积分效应因此在瞬态过程分析中时间总是表示实际的时序 28. 析类型和分析选项在第一个载荷步后也就是在你发出你的第一个SOLVL命令之后不能被改变 全NROPTFNLL程序使用完全的牛顿拉普森处理方法在这种处理方法中每进行一次平衡迭代修改刚度矩阵一次，如果自适应下降是关闭的，程序每一次平衡迭代都使用正切刚度矩阵，我们一般不建议关闭自适应下降，但是你或许发现这样做可能更有效，如果自适应下降是打开的，缺省只要迭代保持稳定也就是只要残余项减小且没有负主对角线出现，程序将仅使用正切刚度阵。如果在一次迭代中探测到发散倾向，程序抛弃发散的迭代且重新开始求解，应用正切和正割刚度矩阵的加权组合，当迭代回到收敛模式时程序将重新开始使用正切刚度矩阵，对复杂的非线性问题自适应下降通常将提高程序获得收敛的能力。 修正的NROPTMODI程序使用修正的牛顿拉普森方法，在这种方法中正切刚度矩阵在每一子步中都被修正，在一个子步的平衡迭代期间矩阵不被改变，这个选项不适用于大变形分析，自适应下降是不可用的 初始刚度NROPTINIT程序在每一次平衡迭代中都使用初始刚度矩阵这一选项比完全选项似乎较不易发散，但它经常要求更多次的迭代来得到收敛，它不适用于大变形分析，自适应下降是不可用的 29. 使用严格的收敛准则将提高你的结果的精度，但以多更次的平衡迭代为代价。如果你想严格加放松你的准则你应当改变TOLER（缺省是0.001）两个数量级，一般地你应当继续使用VALUE的缺省值，也就是通过调整TOLER而不是VALUL 改变收敛准则，你应当确保MINREF=1.0的缺省值在你的分析范围内有意义 30. 线搜索选项LNSRCH 这个选项是对自适应下降的替代当被激活时无论何时发现硬化响应这个收敛提高工具用程序计算出的比例因子具有0和1之间的值乘以计算出的位移增量因为线搜索算法是用来对自适应下降选项NROPT进行的替代如果线搜索选项是开自适应下降不被自动激活不建议你同时激活线搜索和自适应下降 31. 你可以通过产生一个abort文件Jobname.abt停止一个非线性分析，一旦求解成功地完成或者收敛失败发生,程序也将停止分析,如果一个分析在终止前已成功地完成了一次或多次迭代,你可以屡次重启动它. 32. 由于屈服点和比例极限相差很小，因此在ANSYS程序中假定它们相同。在应力一应变的曲线中低于屈服点的叫作弹性部分，超过屈服点的叫作塑性部分，也叫作应变强化部分。塑性分析中考虑了塑性区域的材料特性 。 33. 等向强化是指屈服面以材料中所作塑性功的大小为基础在尺寸上扩张，对Mises屈服准则来说屈服面在所有方向均匀扩张，由于等向强化，在受压方向的屈服应力等于受拉过程中所达到的最高应力 。随动强化假定屈服面的大小保持不变而仅在屈服的方向上移动，当某个方向的屈服应力升高时其相反方向的屈服应力应该降低，随动强化中由于拉伸方向屈服应力的增加导致压缩方向屈服应力的降低，所以在对应的两个屈服应力之间总存一个的差值2σy初始各向同性的材料在屈服后将不再是向同性的。 34. 如果还在进行大应变分析应力应变曲线数据应该是真实应力真实应变 35. 对双线性选项BKIN、BISO，可以按下述方法来决定σy 、Et。如果材料没有明显的屈服应力σy通常以产生0.2%的塑性应变所对应的应力作为屈服应力，而Et可以通过在分析中所预期的应变范围内来拟合实验曲线得到 36. 在塑性分析中对每个节点都可以输出下列量 EPPL塑性应变分量 EPEQ累加的等效塑性应变 SEPL根据输入的应力应变曲线估算出的对于EPEQ的等效应力 HPRES静水压应力 PSV塑性状态变量 PLWK单位体积内累加的塑性功 37. 如果一个单元的所有积分点都是弹性的EPEQ＝0，那么节点的弹性应变和应力从积分点外插得到。如果任一积分点是塑性的EPEQ>0，那么节点的弹性应变和应力实际上是积分点的值。这是程序的缺省情况，但可以人为的改变它 。 38. 缓慢加载应该保证在一个时间步内最大的塑性应变增量小于5%，一般来说如果Fy是系统刚开始屈服时的载荷，那么在塑性范围内的载荷增量应近似为0.05*Fy (对用面力或集中力加载的情况 )；Fy（对用位移加载的情况）。 39. 为了得到可接受的结果，对真实应变超过50%的塑性分析应使用大应变单元（VISCO106、107及108 ）。 40. 大应变分析的任何迭代中低劣的单元形状，也就是大的纵横比、过度的顶角以及具有负面积的已扭曲单元将是有害的。ANSYS程序对于求解中遇到的低劣单元形状不发出任何警告，必须进行人工检查。 41. 内应力和横向刚度之间的联系通称为应力刚化。ANSYS程序通过生成和使用一个称作应力刚化矩阵的辅助刚度矩阵来考虑应力刚化效应，尽管应力刚度矩阵是使用线性理论得到的，但由于应力（应力刚度矩阵）在每次迭代之间是变化的这个事实，因而它是非线性的。大变形分析中（NLGEOM　ON）包含应力刚化效应（SSTIF　ON）将把应力刚度矩阵加到主刚度矩阵上，以在具有大应变或大挠度性能的大多数单元中产生一个近似的协调切向刚度矩阵。 42. 对于大多数实体单元应力刚化的效应是与问题相关的，在大变型分析中的应用可能提高也可能降低收敛性。在大多数情况下，首先应该尝试一个应力刚化效应OFF的分析，如果你正在模拟一个受到弯曲或拉伸载荷的薄的结构，当用应力硬化OFF关时遇到收敛困难，则尝试打开应力硬化 。 43. 考虑到经受塑性变形的区域要求一个合理的积分点密度，每个低阶单元将提供和高阶单元所能提供的一样多积分点数，因此经常优先用于塑性分析。在重要塑性区域网格密度变得特别地重要，因为大挠度要求对于一个精确的解个单元的变形弯曲不能超过30度。 44. 通常你应当避免和弧长方法一起使用JCG或者PCG求解器，因为弧长方法可能会产生一个负定刚度矩阵（负的主对角线），用这些求解器其可能导致求解失败。在任何载荷步的开始你可以从Newton-Raphson迭代方法到弧长方法自由转换，然而要从弧长到Newton-Raphson迭代转换，你必须终止分析然后重起动，且在重起动的第一个载荷步中去杀死弧长方法ARCLEN　OFF。 45. 点─点接触单元主要用于模拟点─点的接触行为，为了使用点─点的接触单元，你需要预先知道接触位置，这类接触问题只能适用于接触面之间有较小相对滑动的情况。 46. 点─面接触单元主要用于给点─面的接触行为建模，例如两根梁的相互接触。如果通过一组结点来定义接触面生成多个单元，那么可以通过点─面的接触单元来模拟面─面的接触问题。面即可以是刚性体也可以是柔性体，这类接触问题的一个典型例子是插头到插座里。使用这类接触单元不需要预先知道确切的接触位置，接触面之间也不需要保持一致的网格，并且允许有大的变形和大的相对滑动 。 47. 对使用Targe169和Conta171或Conta172来定义2-D接触对，使用Targe170和Conta173或Conta174来定义3-D接触对。 48. 你能够使用基本几形状来模拟目标面，例如圆、圆柱、圆锥球。直线、抛物线、弧线和三角形不被允许，虽然你不能把这些基本原型彼此合在一起，或者是把它们和其它的目标形状合在一起，以便形成一个同一实常数号的复杂目标面，但你可以给每个基本原型指定它自己的实常的号。 49. 粗的网格离散可能导致收敛问题，如果刚性面有一个实的凸角，求解大的滑动问题时很难获得收敛结果，为了避免这些建模问题，在实体模型上使用线或面的倒角来使尖角光滑化，或者在曲率突然变化的区域使用更细的网格 。 50. 注意不能使用镜面对称技术（ARSYSM，LSYMM）来映射圆、圆柱、圆锥或球面到对称平面的另一边，因为每个实常数的设置不能同时赋给多个基本原型段。 51. 目标面的结点号顺序是重要的，因为它定义了接触主向。对2─D接触问题当沿着目标线从第一个结点移向第二个结点时变形体的接触单元必须位于目标面的右边，对3─D接触问题目标三角形单元号应该使刚性面的外法线方向指向接触面，外法线通过右手原则来定义。 52. 程序通过组成变形体表面的接触单元来定义接触表面，接触单元与下面覆盖的变形体单元有同样的几何特性，接触单元与下面覆盖的变形体单元必须处于同一阶次。 53. CONTA171这是一种2─D2个结点的低附线单元可能位于2─D实体壳或梁单元的表面 CONTA172这是一个2─D的3结点的高阶抛物线形单元可能位于有中结点的2─D实体或梁单元的表面 CONTA173这是一个3─D的4结点的低阶四边形单元可能位于3─D实体或壳单元的表面它可能褪化成一个结点的三角形单元 CONTA174这是一个3─D8结点的高阶四边形单元可能位于有中结点的3─D实体或壳单元的表面它可能褪化成6结点的三角形单元 54. 置每个接触对的接触面和目标面必须有相同的实常数号，而每个接触对必须有它自己不同的实常数号。 55. 控制面－面接触单元接触行为的实常数FKN、FTOLN、ICONT、PINB、PMAX和PMIN既可以定义一个正值，也可以定义一个负值，程序将正值作为比例因子，将负值作为真实值。 56. 对面─面的接触单元程序可以使用扩增的拉格朗日算法或罚函数方法，通过使用单元关键字KETOPT2来指定 ，扩张的拉格朗日算法是为了找到精确的拉格朗日乘子而对罚函数修正项进行反复迭代，与罚函数的方法相比拉格朗日方法不易引起病态条件，对接触刚度的灵敏度较小，然而在有些分析中扩增的拉格朗日方法可能需要更多的迭代，特别是在变形后网格变得太扭曲时 ，使用拉格朗日算法的同时应使用实常数FTOLN。 57. 所有的接触问题都需要定义接触刚度，两个表面之间渗量的大小取决于接触刚度，过大的接触刚度可能会引起总刚矩阵的病态而造成收敛困难，一般应该选取足够大的接触刚度以保证接触渗透小到可以接受，但同时又应该让接触刚度足够小以使不会引起总刚矩阵的病态问题而保证收敛性。 58. 弹性库仑摩擦允许存在粘合和滑动状态粘合区被当作一个刚度为KT的弹性区来处理在变形期间当接触面是粘合而不是滑动的时候选择这种摩擦类型是好的刚性库仑行为仅仅允许有滑动摩而接触面不能粘合仅仅在两个面处理持续的相对滑动时才选择这种摩擦类型如果运动停止或逆转将会遇到收敛性的问题 59. Table 2.2. ANSYS File types and Formats File Type File Name File Format Log file Jobname.LOG ASCII Error file Jobname.ERR ASCII Output file Jobname.OUT ASCII Database file Jobname.DB Binary Results file: structural or coupled thermal magnetic FLOTRAN Jobname.xxx Jobname.RST Jobname.RTH Jobname.RMG Jobname.RFL Binary Load step file Jobname.Sn ASCII Graphics file Jobname.GRPH ASCII (special format) Element matrices Jobname.EMAT Binary 60. Commands that begin with a slash ( / ) usually perform general program control tasks, such as entry to routines, file management, and graphics controls. Commands that begin with a star ( * ) are part of the ANSYS Parametric Design Language (APDL). 61. Real number values input to integer data fields will be rounded to the nearest integer. The absolute value of integer data must fall between zero and 99,999,999. 62. The acceptable range of values for real data is +/-1.0E+60 to +/-1.0E-60. No exponent can exceed +60 or be less than -60. The program accepts real numbers in integer fields, but rounds them to the nearest integer. You can specify a real number using a decimal point (such as 327.58) or an exponent (such as 3.2758E2). The E (or D) character, used to indicate an exponent, may be in upper or lower case. This limit applies to all ANSYS input commands, regardless of platform. 63. ANSYS interprets numbers entered for Angle arguments as degrees. Note that there are functions in ANSYS that could use radians if the *AFUN command had been used. 64. If an abbreviation that you set matches an ANSYS command, the abbreviation overrides the command. Therefore, use caution in choosing abbreviation names. 65. You can record a frequently used sequence of ANSYS commands in a macro file, thus creating a personalized ANSYS command. If you enter a command name that ANSYS does not recognize, it searches for a macro file by that name (with an extension of .MAC or .mac). If the file exists, ANSYS executes it.On Unix and Windows systems, the ANSYS program searches for macro files in the following order: 1---ANSYS looks first in the ANSYS documentation directory.2---It then looks at the directories that have been defined for the environmental variable ANSYS_MACROLIB. You can set up the ANSYS_MACROLIB variable after the installation of ANSYS software and before the program is started.3---Next, on Unix systems, ANSYS looks in /PSEARCH or in the login directory. On Windows systems, it looks in /PSEARCH or in the home directory.4--Finally, ANSYS looks in the current or working directory 66. Some menu topics automatically expand to show their contents. To disable this feature, set the ANSYS_MENUEXP environment variable to 0. 67. Users can change the menu hierarchy of the Main Menu. You can customize it to your needs by using the User Interface Design Language (UIDL), an ANSYS-developed GUI language 68. Real number values input to integer data fields will be rounded to the nearest integer. The absolute value of integer data must fall between zero and 99,999,999. 69. The acceptable range of values for real data is +/-1.0E+60 to +/-1.0E-60. 70. ANSYS interprets numbers entered for Angle arguments as degrees. Note that there are functions in ANSYS that could use radians if the *AFUN command had been used. 71. The abbreviation must begin with a letter and should not have any spaces. If an abbreviation that you set matches an ANSYS command, the abbreviation overrides the command. Therefore, use caution in choosing abbreviation names. You can abbreviate up to 60 characters, and up to 100 abbreviations are allowed per ANSYS session. -b list or nolist Activates the ANSYS program in batch mode. The options -blist or -b by itself cause the input listing to be included in the output. The -bnolist option causes the input listing not to be included. For more information about running ANSYS in batch mode, see Interactive Versus Batch Mode. -d device Specifies the type of graphics device. This option applies only to interactive mode. For UNIX systems, graphics device choices are X11, X11C, or 3D. For Windows systems, graphics device options are WIN32 or WIN32C, or 3D. -db value Defines the portion of workspace (memory) to be used for the database. The defaults for UNIX and Windows are 64 and 32 megabytes, respectively. -dtm Enables the Drop Test Module (DTM) advanced task (add-on). The DTM is an optional add-on feature to the ANSYS/LS-DYNA product which simplifies the procedure for simulating a drop test. This option is only valid if you have a license for the DTM. See Drop Test Module in the ANSYS/LS-DYNA User's Guide for more information. -f option Sets ANSYS to run in fixed-memory mode. The nogrow option sets ANSYS to use a fixed-mode memory addressing scheme. The no or off options set ANSYS to use dynamic memory allocation for scratch memory as needed (default setting). If you do not set any arguments, ANSYS uses fixed-mode memory allocation for scratch memory, but allows other sections of the ANSYS work space to grow as required. -g Launches the ANSYS program with the Graphical User Interface (GUI) on. If you select this option, an X11 graphics device is assumed for UNIX unless the -d option specifies a different device. This option is not used on Windows systems. To activate the GUI once ANSYS has started, you need to enter two commands in the ANSYS input window: /SHOW to define the graphics device, and /MENU,ON to activate the GUI. The -g option is valid only for interactive mode. Note:If you start ANSYS via the -g option, the program ignores any /SHOW command in the start61.ans file and displays a splash screen briefly before opening the GUI windows. -gs Launches the ANSYS program with the Mechanical Toolbar interface on. -j Jobname Specifies the initial jobname, a name assigned to all files generated by the program for a specific model. If you omit the -j option, the jobname is assumed to be file. -l language Specifies a language file to use other than US English. This option is valid only if you have a translated message file in an appropriately named subdirectory in /ansys_inc/ansys61/docu (or \ansys_inc\ansys61\docu on Windows systems). -m workspace Specifies the total size of the workspace (memory) in megabytes. If you omit the -m option, the default is 128 megabytes for UNIX and 64 megabytes for Windows. -name value Defines ANSYS parameters at program start-up. The parameter name must be at least two characters long. For details about parameters, see the ANSYS Modeling and Meshing Guide. -p productname Defines which ANSYS product will run during the session (ANSYS/Multiphysics, ANSYS/Structural, etc.). For more detailed information about the -p option, see Choosing an ANSYS Product. -pp Enables the Parallel Performance for ANSYS advanced task (add-on). When Parallel Performance for ANSYS is licensed, you can specify two multiprocessor solver options from the EQSLV command: AMG and DOMAIN. AMG initiates the Algebraic Multigrid solver (AMG) and DOMAIN initiates the Distributed Domain Solver (DDS). The -pp option is valid only if you have a license for Parallel Performance for ANSYS. See Solution in the ANSYS Basic Analysis Guide for more information about solver selection. See Improving ANSYS Performance and Parallel Performance for ANSYS in the ANSYS Advanced Analysis Techniques Guide for more information about these Parallel Performance for ANSYS solvers. -s read or noread Specifies whether the program reads the start61.ans file at start-up. If you omit the -s option, ANSYS reads the start61.ans file in interactive mode and not in batch mode. -v Returns the ANSYS release number, update number, copyright date, and license manager version number. 72. Notes About Solid-Model Loads As mentioned earlier, solid-model loads are automatically transferred to the finite element model at the beginning of solution. If you mix solid model loads with finite-element model loads, couplings, or constraint equations, you should be aware of the following possible conflicts: 1.Transferred solid loads will replace nodal or element loads already present, regardless of the order in which the loads were input. for example, DL,,,UX on a line will overwrite any D,,,UX's on the nodes of that line at transfer time. 2.Deleting solid model loads also deletes any corresponding finite element loads. For example, SFADELE,,,PRES on an area will immediately delete any SFE,,,PRES's on the elements in that area. 3.Line or area symmetry or antisymmetry conditions (DL,,,SYMM, DL,,,ASYM, DA,,,SYMM, or DA,,,ASYM) often introduce nodal rotations that could effect nodal constraints, nodal forces, couplings, or constraint equations on nodes belonging to constrained lines or areas. 73. You need to be aware of the possibility of conflicting DK, DL, and DA constraint specifications and how the ANSYS program handles them. The following conflicts can arise: 1. A DL specification can conflict with a DL specification on an adjacent line (shared keypoint). 2. A DL specification can conflict with a DK specification at either keypoint. 3. A DA specification can conflict with a DA specification on an adjacent area (shared lines/keypoints). 4. A DA specification can conflict with a DL specification on any of its lines. 5. A DA specification can conflict with a DK specification on any of its keypoints. Accordingly, for conflicting constraints, DK commands overwrite DL commands and DL commands overwrite DA commands. For conflicting constraints, constraints specified for a higher line number or area number overwrite the constraints specified for a lower line number or area number, respectively. The constraint specification issue order does not matter. For conflicting constraints on flow degrees of freedom VX, VY, or VZ, zero values (wall conditions) are always given priority over non-zero values (inlet/outlet conditions). "Conflict" in this situation will not produce a warning. 74. Because the solution phase generally requires more computer resources that the other phases of an analysis, it is better suited to batch (background) mode than interactive mode. The solver writes output to the output file (Jobname.OUT) and the results file. If you run the solution interactively, the output "file" is actually your screen (window). Another useful file produced during solution is Jobname.STAT, which gives the status of the solution. You can use this file to monitor an analysis while it is running. It is particularly useful in iterative analyses such as nonlinear and transient analyses. 75. Typically, you would set the effective Poisson's ratio to the input Poisson's ratio for elastic equivalent strain (item and component EPEL,EQV) and to 0.5 for inelastic strains (item and component EPPL,EQV or EPCR,EQV). For total strains (item and component EPTOT,EQV), you would typically use an effective Poisson's ratio between the input Poisson's ratio and 0.5. As an alternative, you can save the equivalent elastic strains using ETABLE with the effective Poisson's ratio equal to the input Poisson's ratio and save the equivalent plastic strains in another table using 0.5 as the effective Poisson's ratio, then combine the two table entries using SADD to obtain the total equivalent strain. 76. You can use the fact that ANSYS does not update the element table automatically after a new SET command to good advantage: for example, to compare element results between two or more load steps, or even between two or more analyses. 77. The averaging calculations for PowerGraphics include results for only the model surface. The averaging calculations, plots, and listings for the Full Model method include results for the entire model (interior and exterior surfaces). Therefore, the PowerGraphics and Full Model methods display results values differently for nodal results (but not for element results). 78. The program automatically multiplies the displacements in your results display, so that their effect will be more readily apparent. You can adjust this multiplication factor, using the /DSCALE command (Utility Menu> PlotCtrls> Style> Displacement Scaling). The program interprets exactly zero values of this multiplier (DMULT = 0) as the default setting, which causes the displacements to be scaled automatically to a readily discernible value. Thus, to obtain "zero" displacements (that is, an undistorted display) you must set DMULT = OFF. 79. Isosurface displays are surfaces of constant values (for example, stress). To obtain an isosurface display of Von Mises stress, perform these steps: 1) Issue the command /CTYPE,1 (Utility Menu> PlotCtrls> Style> Contours> Contour Style). 2) Issue the command PLNSOL,S,EQV (Main Menu> General Postproc> Plot Results> Contour Plot> Nodal Solu). You can animate isosurfaces. To do so, either invoke the ANISOS macro (Utility Menu> PlotCtrls> Animate> Isosurfaces). 80. Text annotation can be applied either as stroke text (line-draw characters created within ANSYS) or as bitmap fonts. Bitmap fonts are available on most systems, with the number and type varying from system to system. Bitmap fonts must be enabled (Utility Menu> PlotCtrls> Annotation> Enable Bitmap Font) before the annotation is created. You cannot use the “!” and “$” characters in ANSYS text annotation. 4.2. Prerequisites for Adaptive Meshing The ANSYS program includes a prewritten macro, ADAPT.MAC, to perform adaptive meshing. Your model must satisfy certain preconditions before you can successfully activate the ADAPT macro. (In some cases, models that do not conform to these criteria can be adaptively meshed using a modified procedure, as discussed below.) These requirements include the following: · The standard ADAPT procedure is valid only for single-solution linear static structural and linear steady-state thermal analyses. · Your model should preferably use only one material type, as the error calculations are based in part on average nodal stresses, and would thus often be invalid at the material interfaces. Also, an element's error energy is affected by its elastic modulus. Therefore, even if the stress discontinuity is the same in two adjoining elements, their error energy will be different if they have different material properties. You should also avoid abrupt changes in shell thickness, as such discontinuities will cause similar stress-averaging problems. · Your model must use element types that support error calculations. (See Element Types That can be Used in Adaptive Meshing for a list of valid element types.) · You must build your model using meshable solid model entities: that is, characteristics that will cause meshing failure must not be built into your model. Table 4.1. Element Types That Can Be Used in Adaptive Meshing Type Element Description 2-D Structural Solids PLANE2 PLANE25 PLANE42 PLANE82 PLANE83 2-D 6-Node Triangular Solid Axisymmetric Harmonic Solid 2-D 4-Node Isoparametric Solid 2-D 8-Node Solid Axisymmetric Harmonic 8-Node Solid 3-D Structural Solids SOLID45 SOLID64 SOLID92 SOLID95 3-D 8-Node Isoparametric Solid 3-D Anisotropic Solid 3-D 10-Node Tetrahedral Solid 3-D 20-Node Isoparametric Solid 3-D Structural Shells SHELL43 SHELL63 SHELL93 Plastic Quadrilateral Shell Elastic Quadrilateral Shell 8-Node Isoparametric Shell 2-D Thermal Solids PLANE35 PLANE75 PLANE55 PLANE77 PLANE78 2-D 6-Node Triangular Solid Axisymmetric Harmonic Solid 2-D 4-Node Isoparametric Solid 2-D 8-Node Solid Axisymmetric Harmonic 8-Node Solid 3-D Thermal Solids SOLID70 SOLID87 SOLID90 3-D 8-Node Isoparametric Solid 3-D 10-Node Tetrahedral Solid 3-D 20-Node Isoparametric Solid 3-D Thermal Shells SHELL57 Plastic Quadrilateral Shell If you select a set of areas or volumes, the ADAPT macro will adjust element sizes only in those regions that are in the selected set. You will have to mesh your entire model in PREP7 before executing ADAPT. If you desire to mesh both volumes and areas, you can create a user subroutine, ADAPTMSH.MAC, to perform all the desired operations. You will need to clear any specially-meshed entities before remeshing. Such a subroutine might look like this: C*** Subroutine ADAPTMSH.MAC - Your name - Job Name - Date Created TYPE,1 ! Set element TYPE attribute for area meshing ACLEAR,3,5,2 ! Clear areas and volumes to be meshed by this subroutine VCLEAR,ALL AMESH,3,5,2 ! Mesh areas 3 and 5 (no other areas will be meshed by ADAPT) TYPE,2 ! Change element type for volume mesh VMESH,ALL ! Mesh all volumes Please see the TYPE, ACLEAR, VCLEAR, AMESH, and VMESH command descriptions for more information. We strongly recommend that you include a comment line (C***) to identify your macro uniquely. This comment line will be echoed in the job printout, and will provide assurance that the ADAPT macro has used the correct user subroutine. 81. Linear Elements (No Midside Nodes) , For structural analyses, these corner noded elements with extra shape functions will often yield an accurate solution in a reasonable amount of computer time. When using these elements, it is important to avoid their degenerate forms in critical regions. That is, avoid using the triangular form of 2-D linear elements and the wedge or tetrahedral forms of 3-D linear elements in high results-gradient regions, or other regions of special interest. You should also take care to avoid using excessively distorted linear elements. In nonlinear structural analyses, you will usually obtain better accuracy at less expense if you use a fine mesh of these linear elements rather than a comparable coarse mesh of quadratic elements. 82. When modeling a curved shell, you must choose between using curved (that is, quadratic) or flat (linear) shell elements. Each choice has its advantages and disadvantages. For most practical cases, the majority of problems can be solved to a high degree of accuracy in a minimum amount of computer time with flat elements. You must take care, however, to ensure that you use enough flat elements to model the curved surface adequately. Obviously, the smaller the element, the better the accuracy. It is recommended that the 3-D flat shell elements not extend over more than a 15° arc. Conical shell (axisymmetric line) elements should be limited to a 10° arc (or 5° if near the Y axis). 83. For most non-structural analyses (thermal, magnetic, etc.), the linear elements are nearly as good as the higher order elements, and are less expensive to use. Degenerate elements (triangles and tetrahedra) usually produce accurate results in non-structural analyses. 84. Quadratic Elements (Midside Nodes) 85. For linear structural analyses with degenerate element shapes (that is, triangular 2-D elements and wedge or tetrahedral 3-D elements), the quadratic elements will usually yield better results at less expense than will the linear elements. However, in order to use these elements correctly, you need to be aware of a few peculiar traits that they exhibit: One-element meshes of higher-order quadrilateral elements such as PLANE82 and SHELL93 may produce a singularity due to zero energy deformation. In postprocessing, the program uses only corner nodes for section and hidden line displays. Similarly, nodal stress data for printout and postprocessing are available only for the corner nodes. In graphics displays, midside node elements, which actually use a curved edge in the element formulation, are displayed with straight-line segments (unless PowerGraphics is used). Models will therefore look "cruder" than they actually are. A quadratic element has no more integration points than a linear element. For this reason, linear elements will usually be preferred for nonlinear analyses. 86. You must be careful when you directly join elements that have differing degrees of freedom (DOFs), because there will be inconsistencies at the interface. When elements are not consistent with each other, the solution may not transfer appropriate forces or moments between different elements. To be consistent, two elements must have the same DOFs; for example, they must both have the same number and type of displacement DOFs and the same number and type of rotational DOFs. Furthermore, the DOFs must overlay (be tied to) each other; that is, they must be continuous across the element boundaries at the interface. 87. Models of axisymmetric 3-D structures may be represented in equivalent 2-D form. You may expect that results from a 2-D axisymmetric analysis will be more accurate than those from an equivalent 3-D analysis. 88. By definition, a fully axisymmetric model can only be subjected to axisymmetric loads. In many situations, however, axisymmetric structures will experience non-axisymmetric loads. You must use a special type of element, known as an axisymmetric harmonic element, to create a 2-D model of an axisymmetric structure with non-axisymmetric loads. See Axisymmetric Elements with Nonaxisymmetric Loads in the ANSYS Elements Reference for details. 89. Special requirements for axisymmetric models include: The axis of symmetry must coincide with the global Cartesian Y-axis. Negative nodal X-coordinates are not permitted. The global Cartesian Y-direction represents the axial direction, the global Cartesian X-direction represents the radial direction, and the global Cartesian Z-direction corresponds to the circumferential direction. Your model should be assembled using appropriate element types: For axisymmetric models, use applicable 2-D solids with KEYOPT(3) = 1, and/or axisymmetric shells. In addition, various link, contact, combination, and surface elements can be included in a model that also contains axisymmetric solids or shells. (The program will not realize that these "other" elements are axisymmetric unless axisymmetric solids or shells are present.) If the ANSYS Elements Reference does not discuss axisymmetric applications for a particular element type, do not use that element type in an axisymmetric analysis. For axisymmetric harmonic models, use only axisymmetric harmonic elements. SHELL51 and SHELL61 elements cannot lie on the global Y-axis. For models containing 2-D solid elements in which shear effects are important, at least two elements through the thickness should be used. 90. When you define a keypoint or a node, the program response labels the coordinates as X, Y, and Z, regardless of which coordinate system is active. You should make the appropriate mental substitutions if the active coordinate system is not Cartesian (R, θ, Z for cylindrical and R, θ, Φ for spherical or toroidal). 91. While global and local coordinate systems locate geometry items, the nodal coordinate system orients the degree of freedom directions at each node. Each node has its own nodal coordinate system, which, by default, is parallel to global Cartesian (regardless of the active coordinate system in which the node was defined). In POST1, results data are reported in terms of the results coordinate system [RSYS], not the nodal coordinate system. 92. Every element has its own coordinate system, the element coordinate system, that determines the direction of orthotropic material properties, applied pressures, and results (such as stresses and strains) for that element. All element coordinate systems are right-handed orthogonal systems. The default orientations for most elements' coordinate systems fit the following patterns: 1) Line elements usually have the element X-axis directed from their node I toward their node J. 2)Shell elements usually have the element X-axis similarly directed (from I toward J), the Z-axis normal to the shell surface (with the positive direction determined by the right-hand rule around the element from node I to J to K), and the Y-axis perpendicular to the X and Z axes. 3) For 2-D and 3-D solid elements, the element coordinate system is usually parallel to the global Cartesian system. However, not all elements correspond to these patterns; see specific element descriptions in the ANSYS Elements Reference for the default element coordinate system orientation for such elements. 93. An existing entity that you want to pick might lie close to, but not exactly on, your working plane. By specifying a retrieval tolerance with the WPSTYL command or GUI path, you can instruct the program to consider entities that are within that tolerance to be on the working plane. This tolerance, in effect, gives "thickness" to your working plane, for retrieval picking purposes. 94. working planes are completely separate from coordinate systems. When you change or move the working plane, for instance, the coordinate system does not change to reflect the new working plane type or location. This can be frustrating if you are using a combination of picking (based on the working plane), and keyboard input of entities such as keypoints (based on active coordinate system). For instance, if you move the working plane from its default position, then wish to define a keypoint at the new origin of the working plane with keyboard input (that is K,1205,0,0,0), you'll find that the keypoint is located at the coordinate system origin rather than the working plane origin. If you find yourself forcing the active coordinate system to follow the working plane around as you model, consider using an option on the CSYS command or GUI path to do this automatically. The command CSYS,WP or CSYS,4 will force the active coordinate system to be of the same system type (for example, Cartesian) and in the same location as the working plane. 95. Solid modeling operations in a toroidal coordinate system are not recommended. Areas or volumes generated may not be what you expect. 96. A lower order entity cannot be deleted if it is attached to a higher-order entity. Thus, a volume cannot be deleted if it has been meshed, a line cannot be deleted if it is attached to an area, and so forth. If an entity is attached to any loads, deleting or redefining that entity will delete the attached loads from the database. The hierarchy of modeling entities is as listed below: Highest Elements (and Element Loads)   Nodes (and Nodal Loads)   Volumes (and Solid-Model Body Loads)   Areas (and Solid-Model Surface Loads)   Lines (and Solid-Model Line Loads) Lowest Keypoints (and Solid-Model Point Loads) If you need to revise a solid model after it has been meshed, you must usually first delete all the nodes and elements in the portion of the model to be revised, using the xCLEAR commands 97. Hard points are actually a special type of keypoints. You can use hard points to apply loads or obtain data from arbitrary points on lines and areas within your model. If you issue any commands that update the geometry of an entity, such as Boolean or simplification commands, any hard points associated with that entity are deleted. Therefore, you should add any hard points after completing the solid model. If you delete an entity that has associated hard points, those hard points are either · Deleted along with the entity (if the hard point is not associated with any other entities). · Detached from the deleted entity (if the hard point is associated with additional entities). You cannot manipulate hard points with commands to copy, move, modify, or modify keypoints. Hard points have their own suite of commands and GUI controls. Mapped meshing is not supported when hard points are used. Hard point information cannot be written to the IGES file. The Jobname.cdb file can be written with the CDWRITE,DB option. You can define hard points on existing lines or areas. In both cases, you can define the location of hard points on such entities by Picking (unavailable for models imported from IGES files). Specifying ratios (available for lines only). Specifying global X,Y, and Z coordinates. 98. To copy a portion of an area: Command(s): ASUB GUI: Main Menu> Preprocessor> Modeling> Create> Areas> Arbitrary> Overlaid on Area 99. Keep this information in mind when extruding volumes: If the area that is being extruded (used as the pattern for the resulting volume) with the VROTAT, VEXT, VOFFST, or VDRAG command is meshed (or belongs to a meshed volume), that mesh will be used as a pattern for the mesh of the volume that is created (see Extruding Meshed Areas). (Compare these commands to the VSWEEP command, which is described in Sweeping Volumes.) If you are interested in extruding your mesh, follow these steps: Mesh the area that is to be extruded, dragged, offset, or rotated (using MESH200 elements). Select an appropriate 3-D element type [ET] (match the shape and number of nodes to the MESH200 element). Activate the selection [TYPE]. Specify the desired number of element divisions in the extruded, rotated, or offset direction (NDIV argument on ESIZE command). If using VDRAG, specify the number of element divisions on the drag path line(s) (LESIZE or ESIZE,,NDIV). Issue the VROTAT, VEXT, VOFFST, or VDRAG command. Concatenated areas [ACCAT] or areas that have concatenated lines [LCCAT] cannot be extruded. You can get around the concatenated line limitation by first meshing the area(s), then deleting the concatenated lines, and finally extruding the area(s) into meshed volume(s). If element attributes have been associated with the pattern area via the AATT command, the opposite area generated by the VDRAG, VEXT, VOFFST, or VROTAT operation will also have those attributes (i.e., the element attributes from the pattern area are copied to the opposite area). Note that only the area opposite the pattern area will have the same attributes as the pattern area; the areas adjacent to the pattern area will not. Use the following command to make the generation of meshed volumes from 2-D models easier: Command(s): EXTOPT GUI: Main Menu>Preprocessor> Modeling> Operate> Extrude> Elem Ext Opts Main Menu> Preprocessor> Meshing> Mesh> Volume Sweep> Sweep Opts EXTOPT controls options relating to the generation of volume elements from area elements using the VEXT, VROTAT, VOFFST, VDRAG, and VSWEEP commands. It enables carry-over of material attributes, real constant attributes, and element coordinate system attributes of the pattern area elements to the created volume elements (except for VSWEEP as noted below). 100. Boolean operations are not valid for entities created by concatenation (see How to Mesh Your Solid Model) and that some Boolean operations cannot always be performed on entities that contain degeneracies. (See Solid Model Loads later in this chapter.). you should take care to redefine your element attributes and solid-model loads. Boolean operations cannot be performed on meshed entities. 101. For very narrow (sliver) areas or very thin volumes, such that the ratio of the minimum to the maximum dimension is less than 0.01, the ASUM and VSUM commands can provide erroneous area or volume information. To ensure that such calculations are accurate, make certain that you subdivide such areas and volumes so that the ratio of the minimum to the maximum is at least 0.05. 102. Try to avoid creating geometries that contain degeneracies, if the degeneracy will lie on a potential intersection curve. A few specific examples of such geometries would include: An untruncated cone primitive. (See Cone Surface Maps to a Parametric Square.) A three-sided area that is neither planar nor lies on a constant-coordinate surface in the active coordinate system. (See Examples of Degeneracies (a).) A fillet area [AFILLT] that tapers to a point. (See Examples of Degeneracies(b).) A skinned area [ASKIN] for which two or more guiding lines intersect. (See Examples of Degeneracies (c).) An area or volume created by rotation [AROTAT, VROTAT] about an axis that intersects any of the input entities. (See Examples of Degeneracies (d).) An area or volume created by dragging [ADRAG, VDRAG] along a path that has a center of curvature that intersects any of the input entities. (See Examples of Degeneracies (e).) 103. Try to avoid performing Boolean operations on entities that are tangent to each other. Similarly, try to avoid Boolean operations on entities that have coincident boundaries. If a failure occurs in a series of Boolean operations, try changing the order of operations. If the Boolean operation fails, you may receive an error message suggesting you loosen (increase) the tolerance from the default value of 1.0x10-4 (1.0E-4). This tolerance affects the precision with which Boolean constructions are formed. Sometimes, simply changing this tolerance and reissuing the Boolean command will suffice. At other times, you might find that you need to retrace your steps, recreating the Boolean's input entities using a changed tolerance, before you can successfully proceed with the Boolean operation. Once you have loosened the tolerance and re-executed the operation successfully, you should return the tolerance to its default value. Doing so will assure precise Boolean constructions later in your modeling effort. 104. You must take care not to define an area or volume that crosses over itself. (You might inadvertently create such an entity by means of an ADRAG or VDRAG command, for instance.) The ANSYS program cannot always detect such a defect before meshing, but an area or volume that crosses over itself will usually reveal itself in a meshing failure. 105. Consider creating complex solid models in pieces and combining them using the RESUME command (Utility Menu> File> Resume from) and CDREAD command (Main Menu> Preprocessor> Archive Model> Read) in the preprocessor (PREP7). The following is an example of this procedure: /PREP7 RESUME,MODEL1,DB CDWRITE,SOLID !Write out just solid model (to file.iges) RESUME,MODEL2,DB !Note that this 2nd RESUME clears MODEL1 from the !database and reads MODEL2 CDREAD,SOLID !Reads in the solid model (from file.iges) !Solid models from MODEL1 and MODEL2 are now !in the current database SAVE,MODEL3,DB !Save combined model to separate file FINISH The CDREAD command automatically renumbers new entities to avoid conflicts with other solid model entities that already exist in the database. In addition, this command automatically executes a NUMMRG,KP command to merge duplicate solid-model entities. 106. ANSYS provides the following two options for importing IGES files. Instructions for using these options appear later in this chapter. SMOOTH (NURBS-based or RV52)--This option uses the standard ANSYS geometry database. The SMOOTH option has no capabilities for automatically creating volumes and models imported through this translator will require manual repair. You must use the standard PREP7 geometry tools to repair your model. The topological and geometric repair tools available with the FACETED option are not available for models imported through this translator. FACETED (or RV53) --This option uses a defeaturing database. The conversion includes automatic merging and the creation of volumes to prepare the models for meshing. If the FACETED option encounters problems translating the IGES file, ANSYS will alert you to this and activate a suite of topological and geometric tools designed specifically for interactive repair of imported models. This option is not recommended for large, complex geometries. Always attempt to import the model using the SMOOTH option first. If you cannot repair the imperfections in the model using the tools that are available to you, attempt to import and repair the model using the FACETED option. If the model to be analyzed is very large, use the CAD program's selection capabilities to create several IGES files, each containing a portion of the model. The ANSYS program will use the next available entity number as each file is read. You can then use the PREP7 merge feature (NUMMRG command or menu path Main Menu>Preprocessor>Numbering Ctrls>Merge Items) to merge coincident entities. For the Pro/ENGINEER program, use these additional guidelines: Set the Config.pro option "iges_out_trim_xyz" to "yes." Set the accuracy to 1E-6 and regenerate the model. Duplicate lines and keypoints are possible when transferring a model in from an IGES file. This often happens with CAD models due to the tolerances and practices that they were created with. You sometimes need to "clean up" these solid models with ANSYS commands that merge duplicate entities together (NUMMRG command or menu path Main Menu> Preprocessor> Numbering Ctrls> Merge Items). 107. 6.1.1.2.4. While Writing an IGES File from ANSYS: Set the system of units [/UNITS] before writing the IGES file. This information is captured on the IGES file and is read by many programs that read IGES files. (You cannot access the /UNITS command directly in the GUI.) Select all lower level solid modeling entities before writing the file (ALLSEL,BELOW,ALL or menu path Utility Menu>Select>Everything Below). If you wish to write out a portion of your model, select only those entities (areas) to be written and all corresponding lower level entities (lines and keypoints). Then unselect any higher level entities (volumes) before writing the file. 108. Curved surfaces that are imported using the FACETED option are internally represented by a grid of flat facets. Nodes that are meshed onto those surfaces (on area interiors) may not follow the original surface as accurately as those at keypoints or those interior to lines, nor as accurately as they would if they had been imported using the SMOOTH option. In a few cases, this could adversely affect analysis results. While the FACETED option's defeaturing database provides robust capabilities for simplifying models, you should take advantage of the SMOOTH options import and modeling capabilities to import and repair any imperfections in your model. If you need to further simplify your geometry, you can then defeature the model using the FACETED option's defeaturing CAD repair tools. The following briefly covers the process you should follow when defeaturing a model: 1. Import the IGES file in SMOOTH mode. 2. Repair and enhance the geometry through the creation of geometric primitives and the use of Boolean operations. Do not mesh the model. 3. Save the database created for the imported or created model. 4. Export the model as an ANSYS IGES file. 5. Clear the database using the /CLEAR command (or exit and restart ANSYS). 6. Set IOPTN to FACETED. 7. Import the IGES file you created. Note You cannot revert back to the SMOOTH mode once you import the file. Be sure you have completed all of the modeling you wish to do using the standard ANSYS geometry database before you import using the FACETED option. 8. Simplify geometry (defeature) to remove problem features from the model. 9. Attempt to mesh the model . If you encounter problems in meshing, you may need to further simplify the geometry. 109. A mapped area mesh contains either only quadrilateral or only triangular elements, while a mapped volume mesh contains only hexahedron elements. In addition, a mapped mesh typically has a regular pattern, with obvious rows of elements. If you want this type of mesh, you must build the geometry as a series of fairly regular volumes and/or areas that can accept a mapped mesh. 110. When you use SmartSizing, we recommend that in most cases you specify the desired SmartSizing settings [SMRTSIZE] and then mesh the entire model at once [AMESH,ALL or VMESH,ALL], rather than SmartSizing area by area or volume by volume. This gives SmartSizing the opportunity to reduce element sizes near small features in adjacent regions. However, you should not try to SmartSize in a single operation areas or volumes that just touch (rather than sharing common keypoints, lines, or areas), such as might exist in a model prepared for contact analysis. The near zero proximity can cause SmartSizing to compute very small element sizes and produce an unreasonably fine mesh, with a huge number of nodes and elements. You should mesh each contiguous piece of such a model as a separate group of areas or volumes. 111. Remember that for best results, all areas or volumes should be meshed at the same time. 112. If you need to mesh multiple volumes, you should consider using the AORDER meshing option in the Mesher Opts dialog box (or issuing the MOPT,AORDER,ON command) so your mesh is created in the smallest area first. This helps ensure that your mesh is adequately dense in smaller areas and that the mesh is of a higher quality. 113. For area meshing, a free mesh can consist of only quadrilateral elements, only triangular elements, or a mixture of the two. For volume meshing, a free mesh is usually restricted to tetrahedral elements. Pyramid-shaped elements may also be introduced into the tetrahedral mesh for transitioning purposes. If your chosen element type is strictly triangular or tetrahedral (for example, PLANE2 and SOLID92), the program will use only that shape during meshing. However, if the chosen element type allows more than one shape (for example, PLANE82 or SOLID95), you can specify which shape (or shapes) to use 114. A special type of free meshing, called fan type meshing, is available for certain contact analysis cases that involve the meshing of three-sided areas with the TARGE170 element. When two of the three sides have only one element division, and the third side has any number of divisions, the result will be a fan type mesh. (The LESIZE command is used to set element divisions.) Fan type meshing ensures that ANSYS uses the minimum number of triangles to fill the area, which is important for contact problems.   ·  · TARGE170 · MSHKEYMSHKEY 115. SmartSizing [SMRTSIZE] cannot be used for mapped meshing. Mapped meshing is not supported when hard points are used. 116. For an area to accept a mapped mesh, the following conditions must be satisfied: 1. The area must be bounded by either three or four lines (with or without concatenation). 2. The area must have equal numbers of element divisions specified on opposite sides, or have divisions matching one of the transition mesh patterns (see Transition Patterns). 3. If the area is bounded by three lines, the number of element divisions must be even and equal on all sides. 4. The meshing key must be set to mapped [MSHKEY,1]. This setting results in a mapped mesh of either all quadrilateral elements or all triangle elements, depending on the current element type and/or the setting of the element shape key [MSHAPE]. 5. If your goal is a mapped triangle mesh, you can also specify the pattern ANSYS uses to create the mesh of triangular elements [MSHPATTERN]. If you do not specify a pattern, ANSYS chooses one for you. See the MSHPATTERN command description in the ANSYS Commands Reference for an illustration of the available patterns. If an area is bounded by more than four lines, you can combine [LCOMB] or concatenate [LCCAT] some of the lines to reduce the total number of lines to four. Line divisions cannot be directly assigned to concatenated lines. However, divisions can be assigned to combined lines [LCOMB]. Therefore, there is some advantage to using line combination instead of concatenation. 117. To mesh a volume with all hexahedron elements, the following conditions must be satisfied: 1. The volume must take the shape of a brick (bounded by six areas), wedge or prism (five areas), or tetrahedron (four areas). 2. The volume must have equal numbers of element divisions specified on opposite sides, or have divisions matching one of the transition mesh patterns for hexahedral meshes. See Mapped Volume Meshing for examples of element divisions that will produce a mapped mesh for different volume shapes. Transition mesh patterns for hexahedral meshes are described later in this section. 3. The number of element divisions on triangular areas must be even if the volume is a prism or tetrahedron As with lines, you can add [AADD] or concatenate [ACCAT] areas if you need to reduce the number of areas bounding a volume for mapped meshing. If there are also lines bounding the concatenated areas, the lines must be concatenated as well. You must concatenate the areas first, then follow with line concatenations. The ACCAT command is not supported for models that you import using the IGES defeaturing import function [IOPTN,IGES,FACETED]. However, you can use the ARMERGE command to merge two or more areas in models imported from CAD files. Be aware that when you use the ARMERGE command in this way, locations of deleted keypoints between combined lines are unlikely to have nodes on them! You can create a mapped volume mesh by specifying line divisions on opposite edges of the volume such that the divisions permit a transition mapped hexahedral mesh. Transition mapped hexahedral meshing is only applicable to six-sided volumes (with or without concatenation). Even if you specify free meshing [MSHKEY,0], ANSYS automatically looks for six-sided volumes that match these transition patterns. If a match is found, the volume will be meshed with a transition mapped hexahedral mesh, unless the resulting elements are of poor quality (in which case the mesh will fail). 118. Concatenation is solely intended to be used as an aid to mapped meshing; it is not a Boolean "add" operation. Concatenation should be the last step you undertake before you execute a mapped mesh of your solid model, because the output entity obtained from a concatenation cannot be used in any subsequent solid modeling operation (other than meshing, clearing, or deleting). For example, a line created by an LCCAT operation cannot have any solid model loads applied to it; nor can it be part of any Boolean operation; nor can it be copied, dragged, rotated [xGEN, xDRAG, xROTAT], etc.; nor can it be used in another concatenation. You can readily "undo" a concatenation by simply deleting the line or area produced by the concatenation: · The fastest way to delete concatenated lines or areas is by choosing menu path Main Menu> Preprocessor> Modeling> Delete> Del Concats> Lines or Main Menu> Preprocessor> Modeling> Delete> Del Concats> Areas. Caution When you use this method, ANSYS automatically selects all concatenated lines (or areas) and deletes them without prompting you. · If you want more control over which concatenated lines or areas are selected and deleted, use one of these methods: Command(s): LSEL,Type,LCCA,,,,,KSWP or ASEL,Type,ACCA,,,,,KSWP GUI: Utility Menu>Select>Entities If you are using the Select Entities dialog box, choose both Lines and Concatenated to select concatenated lines. Choose both Areas and Concatenated to select concatenated areas. If desired, use the other controls in the dialog box to refine your selection. You can then delete all of the selected lines or areas [LDELE,ALL or ADELE,ALL] as necessary. Although you need to be aware of the restrictions on output entities listed earlier in this section, no such restrictions affect the input entities in a concatenation. However, the input entities will become "lost" or "detached," so far as higher-level entities are concerned. That is, if an area is bounded by five lines (L1-L5), and two of those lines are concatenated (LCCAT,1,2 >L6), the program will no longer recognize lines L1 and L2 as being attached to that area. However, you can reattach L1 and L2 to the area by deleting L6 to undo the concatenation. (See Input Lines in a Concatenation.) Input lines in a concatenation become detached until the concaternation is undone 119. If you are meshing multiple volumes or areas at one time, you should consider using the meshing option By Size (or issuing the MOPT,ORDER,ON command) so the mesh is created in the smallest volume or area first. This helps ensure that your mesh is adequately dense in smaller volumes or areas and that the mesh is of a higher quality. 120. Generating an Interface Mesh for Gasket Simulations 1. Define interface and structural elements that have corresponding characteristics see table below). 2. Mesh the structural component element that contains the source face using either the AMESH or VMESH command. 3. Mesh the gasket layer component element using either IMESH,LINE or IMESH,AREA; or VDRAG. 4. Mesh the structural component element that contains the target face using either the AMESH or VMESH command. For simulating gasket joints, the interface and structural elements that you choose must have the same characteristics. The following table provides guidelines on choosing compatible elements. For elements with these characteristics: ... use this interface element: ... with one of these structural elements: 2D, linear INTER192 PLANE42, HYPER56, VISCO106, PLANE182 2D, quadratic INTER193 PLANE2, PLANE82, HYPER84, VISCO88, PLANE183 3D, quadratic INTER194 VISCO89, SOLID92, SOLID95, SOLID96, SOLID186, SOLID187 3D, linear INTER195 SOLID45, SOLID46, HYPER58, SOLID62, SOLID64, SOLID65, HYPER86, SOLID185 The IMESH command requires that the target line or area exactly match the source line or area. Also, both target and source lines or areas must be in the same area or volume. As stated in the four step meshing procedure shown above, the area or volume containing the source line or area must be meshed before executing IMESH, while the area or volume containing the target line or area must be meshed after executing IMESH. 121. Picking the STOP button aborts the mesh operation and causes incomplete meshes to be discarded. Areas or volumes that are completely meshed before STOP is picked will be retained. The solid model and finite element model will be left as they were before meshing was initiated. 122. Situations in which we recommend that you turn shape checking off or run it in warning-only mode include: · When you are generating an area mesh [AMESH], but your ultimate intention is to generate a volume mesh [VMESH] of quadratic tetrahedrons with that area as one of the volume's faces. Note that the tetrahedra mesher can fix meshes in which area elements have poor Jacobian ratios. Thus, if you are generating an area mesh for an area that will be a face on a volume in a subsequent volume meshing operation, it may make sense to turn element shape checking to warning-only mode, mesh the area, turn element shape checking on, and then mesh the volume. · When you are importing a mesh [CDREAD]. If "bad" elements exist in a mesh that you want to import and element shape checking is turned on, ANSYS may bring the mesh into the database with "holes" where the bad elements should be (or it may not import the mesh at all). Since neither of these outcomes is desirable, you may want to turn element shape checking either off or to warning-only mode prior to importing a mesh. After you import, we suggest that you turn shape checking back on and recheck the elements [CHECK,ESEL,WARN or CHECK,ESEL,ERR]. Note Once elements are in the database, performing element shape checking will not delete them. If any elements in violation of error limits are selected when you initiate a solution [SOLVE], ANSYS issues an error message and does not process the solution. · When you are using direct generation and you are creating elements that you know will be temporarily invalid. For example, you may be creating a wedge-shaped element that has coincident nodes. You know that you need to merge the coincident nodes [NUMMRG] in order to get valid elements. In this case, it would make sense to turn off element shape checking, complete the desired operations (such as merging nodes in this example), turn element shape checking on, and then check the elements for completeness [CHECK]. 123. 7.5.8.6. Retrieving Element Shape Parameter Data You can use the *GET and *VGET commands to retrieve element shape parameter data: Command(s): *GET, Par, ELEM, ENTNUM, SHPAR, IT1NUM *VGET, ParR, ELEM, ENTNUM, SHPAR, IT1NUM,,, KLOOP Note You cannot use the GUI paths for these commands to retrieve element shape parameter data. For example, the command *GET,A,ELEM,3,SHPAR,ASPE returns the calculated aspect ratio of element number 3 and stores it in a parameter named A. The command *VGET,A(1),ELEM,3,SHPAR,ASPE returns the aspect ratio of element number 3 and stores it in the first location of A. Retrieval continues with elements numbered 4, 5, 6, and so on, until successive array locations are filled. See the descriptions of the *GET and *VGET commands in the ANSYS Commands Reference for more information. 124. You can request improvement of two "types" of tetrahedral elements: · You can request improvement of tetrahedral elements that are not associated with a volume. (Typically, this option is useful for an imported tetrahedral mesh for which no geometry information is attached.) Use one of these methods: Command(s): TIMP GUI: Main Menu> Preprocessor> Meshing> Modify Mesh> Improve Tets> Detached Elems · You can request improvement of tetrahedral elements that are in a selected volume or volumes. (You might want to use this option to further improve a volume mesh created in ANSYS [VMESH].) Use one of these methods: Command(s): VIMP GUI: Main Menu> Preprocessor> Meshing> Modify Mesh> Improve Tets> Volumes 125. The following restrictions apply to tetrahedral mesh improvement: · The mesh must consist of either all linear elements or all quadratic elements. · For all of the elements in the mesh to be eligible for tetrahedral mesh improvement, they must all have the same attributes, including element type. (The element type must be tetrahedral, but the tetrahedral elements may be the degenerated form of hexahedral elements.) After tetrahedral mesh improvement, ANSYS reassigns the attributes from the old set of elements to the new set of elements. Note Tetrahedral mesh improvement is possible in a mesh of mixed element shapes (as opposed to types). For example, as stated earlier, improvement occurs automatically during the creation of transitional pyramid elements at the interface between hexahedral and tetrahedral element types. However, in a mixed mesh, only the tetrahedral elements are improved. · Loading has an effect on whether tetrahedral mesh improvement is possible. Tetrahedral mesh improvement is possible when loading occurs in either of these ways: · When loads have been applied to the element faces or nodes on the boundary of the volume only · When loads have been applied to the solid model (and have been transferred to the finite element mesh) Tetrahedral mesh improvement is not possible when loading occurs in either of these ways: · When loads have been applied to the element faces or nodes within the interior of a volume · When loads have been applied to the solid model (and have been transferred to the finite element mesh), but have also been applied to the element faces or nodes within the interior of a volume Note In the last two loading situations, ANSYS issues a warning message to notify you that you must remove the loads if you want tetrahedral mesh improvement to occur. · If node or element components are defined, you will be asked whether you want to proceed with mesh improvement. If you choose to proceed, you must update any affected components. 126. Cautions · Areas or volumes that are flattened or have a sharp interior corner can commonly experience a meshing failure. · Poor element quality will often occur if you specify too extreme a transition in element sizes. · When using midside-node structural elements to model a curved boundary, you should usually make sure that you make your mesh dense enough that no single element spans more than 15° of arc per element length. If you do not need detailed stress results in the vicinity of a curved boundary, you can force the creation of straight-sided elements [MSHMID,1] in a coarse mesh along curved edges and faces. In cases where a curved-sided element will create an inverted element, the tetrahedra mesher automatically changes it to a straight-sided element and outputs a warning. · A tetrahedron meshing failure can be quite time consuming. One relatively quick way that you can make a preliminary check for a possible tetrahedron meshing failure is by meshing the surfaces of a volume with six-noded triangles. If this surface triangle mesh contains no sudden size transitions (admittedly often a difficult judgement) and produces no curvature or aspect ratio warnings, tetrahedron meshing failure is much less likely than if these conditions are not met. (Be sure to clear or deactivate the triangle elements before using the analysis model.) · Avoid subtracting meshed entities from your model whenever possible. However, if you subtract entities that have been meshed and an undesirable mesh mismatch results, you can recover by clearing the mesh and remeshing the entities. 127. element refinement Value of LEVEL Argument Approximate Edge Length 1 1/2 2 1/3 3 1/4 4 1/8 5 1/9 128. loads and boundary conditions applied at the node and element level (finite element loads) cannot be transferred to new nodes and elements created during refinement. If you have such loads in a region selected for refinement, the program will not allow refinement to take place unless the loads are first deleted. Therefore, it is recommended that you apply loads only to the solid model rather than directly to nodes and elements if you anticipate using mesh refinement. Since solid model loading is not applicable for an explicit dynamics analysis (that is, the ANSYS/LS-DYNA product), mesh refinement must be performed before the application of loads in this type of analysis. 129. The presence of the negative sign affects how ANSYS treats the line divisions if you clear the mesh later (ACLEAR, VCLEAR, etc., or menu path Main Menu>Preprocessor> Meshing> Clear> entity). If the number of line divisions is positive, ANSYS does not remove the line divisions during the clearing operation; if the number is negative, ANSYS removes the line divisions (which will then show up as zeros in a subsequent line listing). 130. Local mesh refinement is not recommended for an explicit dynamics model (that is, when using the ANSYS/LS-DYNA product) since the small elements resulting from refinement may dramatically reduce the time step size. 131. If you are meshing multiple volumes or areas at one time, you should consider using the meshing option By Size (or issuing the MOPT,ORDER,ON command) so the mesh is created in the smallest volume or area first. This helps ensure that your mesh is adequately dense in smaller volumes or areas and that the mesh is of a higher quality. · Line meshing with automatic generation of orientation nodes is supported for elements BEAM4, BEAM24, BEAM44, BEAM161, BEAM188, and BEAM189. If you are meshing a circular arc with beams, and if that arc spans more than 90 degrees, the beam orientation is twisted at the 90-degree point. To prevent the beam orientation from twisting, set the ending orientation keypoint (KE) to be the same as KB, or split the line into 90 degree arcs. After meshing a beam, always use the /ESHAPE,1 command to verify the beam's orientation graphically. You can use the LLIST,,,,ORIENT command to list the selected line(s), along with any assigned orientation keypoints and section data. If you specify one orientation keypoint for a line, ANSYS generates beam elements along the line with a constant orientation. If you specify different orientation keypoints at each end of the line, ANSYS generates a pre-twisted beam. Here one line was divided into two, with the ending orientation keypoint for L1 and the beginning orientation keypoint for L2 being assigned to the same keypoint. A 180° twist is achieved. Since orientation is not required for 2-D beam elements, the beam meshing procedure described in this section does not support 2-D beam elements. · Any operation on a line (copying the line, moving the line, and so on) will destroy the keypoint attributes. · If an orientation keypoint is deleted, ANSYS issues a warning message. · If an orientation keypoint is moved, it remains an orientation keypoint. However, if an orientation keypoint is redefined (K,NPT,X,Y,Z), ANSYS no longer recognizes it as an orientation keypoint. Caution If you issue the CDWRITE command after generating a beam mesh with orientation nodes, the database file will contain all of the nodes for every beam element, including the orientation nodes. However, the orientation keypoints that were specified for the line [LATT] are no longer associated with the line and are not written out to the geometry file. The line does not recognize that orientation keypoints were ever assigned to it, and the orientation keypoints do not "know" that they are orientation keypoints. Thus, the CDWRITE command does not support (for beam meshing) any operation that relies on solid model associativity. For example, meshing the areas adjacent to the meshed line, plotting the line that contains orientation nodes, or clearing the line that contains orientation nodes may not work as expected. This limitation also exists for the IGESOUT command. See the descriptions of the CDWRITE command and the IGESOUT command in the ANSYS Commands Reference for more information. 132. No matter which volume mesher you choose [MOPT,VMESH,Value], it may produce different meshes on different hardware platforms when meshing volumes with tetrahedral elements [VMESH, FVMESH]. 133. Using volume sweeping, you can fill an existing unmeshed volume with elements by sweeping the mesh from a bounding area (called the "source area") throughout the volume. If the source area mesh consists of quadrilateral elements, the volume is filled with hexahedral elements. If the area consists of triangles, the volume is filled with wedges. If the area consists of a combination of quadrilateral and triangular elements, the volume is filled with a combination of hexahedral and wedge elements. The swept mesh is fully associated with the volume. 134. Follow these steps before you invoke the volume sweeper: 1. Determine how many volumes need to be swept by VSWEEP. VSWEEP will sweep either a single volume, all selected volumes (VSWEEP,ALL) or a component of volumes (VSWEEP,CMVL where CMVL is the name of a volume component.) 2. Determine whether the volume's topology can be swept. The volume cannot be swept if any of these statements is true: · If LESIZE is used with the “hard” option, and the source and target areas contain hard division which are the not the same for each respective line, then the volume is not sweepable. · The volume contains more than one shell; in other words, there is an internal void within the volume. (A shell is the volumetric equivalent of an area loop - a set of entities that defines a continuous closed boundary. The SHELL column in a volume listing [VLIST] indicates the number of shells in the volume.) · The source area and the target area are not opposite one another in the volume's topology. (By definition, the target area must be opposite the source area.) · There is a hole in the volume that does not penetrate the source and/or target areas. 135. 看help (Modeling and Meshing Guide(Revising Your Mesh(Refining a Mesh Locally 136. 看help(Modeling and Meshing Guide(Generating the Mesh(Meshing Your Solid Model(Generating a Volume Mesh By Sweeping 137. You must plan ahead to ensure that the interfaces between copied regions will match up node for node. For example, if you freely meshed a volume, the pattern of nodes on the right end would not necessarily match the pattern of nodes on the left end. If the original part and its copy were to be joined such that the right end of one part interfaced with the left end of the other part, a seam of discontinuity would be created where the two mismatched faces touched. It is relatively easy to create matching node patterns along the line edges of meshed areas: simply specify the same number of line divisions and division spacings on both sides of the original part. Volumes are not so straightforward, however. You will need to use a trick to force matching node patterns on two faces of a meshed volume. Before meshing with volume elements, mesh one of the matching faces with dummy area elements, then copy that meshed area to the other matching face. (Depending on how you originally created your volume, you might or might not have some cleaning up to do at this point. If you wind up with duplicate coincident areas, you should redefine your volume in terms of the new meshed area, and delete the original volume.) The volume can then be meshed with solid elements. After the volume meshing is complete, you should delete the dummy area elements. (You can do this fairly cleanly using selecting and either the ACLEAR command or menu path Main Menu> Preprocessor> Meshing> Clear> Areas.). Having created meshed regions which will match up at their interfaces, you can now copy the part, such that the repeated regions just touch. Even though these regions will have matching nodes at the interfaces, the degrees of freedom at these nodes will remain independent; that is, a seam of discontinuity will exist in your model at the interface. You should execute NUMMRG,ALL to eliminate this discontinuity. It is usually good practice to follow these operations with a NUMCMP command (Main Menu> Preprocessor> Numbering Ctrls> Compress Numbers). 138. You cannot use the tools described in this section to change the normal direction of any element that has a body or surface load. We recommend that you apply all of your loads only after ensuring that the element normal directions are acceptable. Caution Real constants (such as non-uniform shell thickness and tapered beam constants) may be invalidated by an element reversal. 139. Two solution methods are available for solving structural problems in the ANSYS family of products: the h-method and the p-method. The h-method can be used for any type of analysis, but the p-method can be used only for linear structural static analyses. Depending on the problem to be solved, the h-method usually requires a finer mesh than the p-method. The p-method provides an excellent way to solve a problem to a desired level of accuracy while using a coarse mesh. 140. Some elements, including those in the 18x family of elements, include stress stiffening effects regardless of the SSTIF command setting. By default, stress stiffening effects are ON when NLGEOM is ON. you may choose to turn stress stiffening OFF for specific problems in which convergence difficulties are seen; for example, local failures. The stress stiffening effects and the prestress effect calculation both control the generation of the stress stiffness matrix, and therefore should not be used together in an analysis. If both are specified, the last option specified will override the previous setting. 141. For a static analysis, the mass matrix formulation you use does not significantly affect the solution accuracy (assuming that the mesh is fine enough). However, if you want to do a prestressed dynamic analysis on the same model, the choice of mass matrix formulation may be important; see the appropriate dynamic analysis section for recommendations. Command(s): LUMPM GUI: Main Menu>Solution>Unabridged Menu>Analysis Options 142. Inertia relief output is stored in the database rather than in the results file (Jobname.RST). When you issue IRLIST, ANSYS pulls the information from the database, which contains the inertia relief output from the most recent solution [SOLVE or PSOLVE]. 143. Vector displays (not to be confused with vector mode) are an effective way of viewing vector quantities, such as displacement (DISP), rotation (ROT), and principal stresses (S1, S2, S3).