| 查看: 3149 | 回复: 7 | ||||
zhuqw金虫 (小有名气)
|
[求助]
热应力耦合失败 已有1人参与
|
|
做激光器工作时候热应力耦合的时候，前面温度部分都算的好好的，到应力部分的时候算了一会程序就崩溃了，ANSYS直接就自动关了，只保存下来了温度的数据。我查看了下错误日志，不知道是不是因为我在求解的时候，在底面施加温度约束的时候用的命令错了？ 我用的是： /SOLU ANTYPE,STATIC TOFFST,273.15 DA,3,TEMP,25 是不是应该改成这样？ /SOLU ANTYPE,STATIC TOFFST,273.15 NSEL,S,LOC,Y,0 D,ALL,TEMP,25 ASEL,ALL 是不是在求解中，都要先选择节点，然后再加载？不能选体或者面或者关键点？ 还有是不是我的网格画的有问题？ 下面是我的错误日志，不知道导致ANSYS崩溃的原因到底是什么 *** WARNING *** CP = 64.834 TIME= 10:06:03 Shape testing revealed that 52605 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 71.370 TIME= 10:06:08 Shape testing revealed that 52605 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 108.249 TIME= 10:06:32 Shape testing revealed that 52605 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 118.748 TIME= 10:06:38 Shape testing revealed that 42585 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 129.450 TIME= 10:06:44 Shape testing revealed that 52605 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 141.914 TIME= 10:06:52 Shape testing revealed that 42585 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 154.550 TIME= 10:06:58 Shape testing revealed that 52605 of the 52605 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 233.768 TIME= 10:07:33 Shape testing revealed that 571 of the 66864 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 426.710 TIME= 10:10:36 Shape testing revealed that 35 of the 962864 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 458.393 TIME= 10:10:56 Shape testing revealed that 43 of the 221575 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 522.213 TIME= 10:11:17 Previous testing revealed that 348841 of the 2141200 selected elements violate shape warning limits. To review warning messages, please see the output or error file, or issue the CHECK command. *** WARNING *** CP = 2510.696 TIME= 10:17:27 Shape testing revealed that 348841 of the 2141200 new or modified elements violate shape warning limits. To review test results, please see the output file or issue the CHECK command. *** WARNING *** CP = 2511.445 TIME= 10:17:27 The ETCHG command has changed some element types. Please examine not only the KEYOPTs, but also the real constants, material properties, boundary conditions, and loadings, and then modify as needed. *** WARNING *** CP = 2514.564 TIME= 10:17:29 Both solid model and finite element model boundary conditions have been applied to this model. As solid loads are transferred to the nodes or elements, they can overwrite directly applied loads. *** WARNING *** CP = 2515.594 TIME= 10:17:29 Constraint on area 3 with inactive load label TEMP not transferred to nodes. *** WARNING *** CP = 2523.332 TIME= 10:17:32 Meshes made up of 10 percent or more of SOLID185 tetrahedra are not recommended. *** WARNING *** CP = 2535.219 TIME= 10:17:33 Previous testing revealed that 348841 of the 2141200 selected elements violate shape warning limits. To review warning messages, please see the output or error file, or issue the CHECK command. |
回复此楼» 猜你喜欢
0860004 求调剂 309分
已经有4人回复
-
材料类284调剂
已经有25人回复
-
一志愿211 0703化学 346分求调剂
已经有5人回复
-
考研调剂-材料类-284
已经有17人回复
-
280求调剂
已经有3人回复
-
0703化学求调剂
已经有18人回复
-
调剂
已经有15人回复
-
复试调剂，一志愿郑州大学材料与化工289分
已经有16人回复
-
349学科化学045106求调剂，化学类都可以
已经有7人回复
-
086003调剂求助
已经有6人回复
» 本主题相关价值贴推荐，对您同样有帮助:
- ansys有限元分析教程
已经有3人回复
shgao20
专家顾问 (职业作家)
-
专家经验: +809 - 仿真EPI: 1
- 应助: 1311 (讲师)
- 金币: 13381.4
- 红花: 267
- 帖子: 3531
- 在线: 473.4小时
- 虫号: 3644138
- 注册: 2015-01-14
- 专业: 动力学与控制
- 管辖: 仿真模拟
【答案】应助回帖
★ ★ ★ ★ ★ ★ ★
感谢参与，应助指数 +1
zhuqw: 金币+7, ★★★很有帮助 2015-12-08 15:50:38
感谢参与，应助指数 +1
zhuqw: 金币+7, ★★★很有帮助 2015-12-08 15:50:38
|
看来主要有两个问题： 1 单元的质量不太好，最差的情况，52605 个单元竟有 52605 个单元超过了质量警告限，而且你使用的 solid185 单元，它退化得到的四节点四面体单元，计算精度很差，最好改为 solid186 单元。 不过，你的单元数多的情况达到百万个，计算模型的规模已经太大了，若改为 solid186 单元，规模 (主要是节点数) 会更大。最好对划分网格改进一下，既要减少不合格单元，又要设法使模型的规模尽量小一点。 2 应力分析时使用 DA,... TEMP,... 和 D,..., TEMP,... 命令是不对的，应力分析时 D 和 DA 命令应该用于位移约束，不能用来施加温度载荷。温度载荷应该使用 BF 族命令 (如 BF、BFA 等) 来施加。 另外，计算中自动退出 ANSYS，应该是计算不收敛造成的，为了避免这一点，可以在求解前执行命令： NCNV,2 这样，计算不收敛时会终止计算但不退出 ANSYS，以便查找问题。 |
2楼2015-11-29 10:53:01
zhuqw
金虫 (小有名气)
- 应助: 2 (幼儿园)
- 金币: 1217.4
- 帖子: 77
- 在线: 74.6小时
- 虫号: 2408038
- 注册: 2013-04-08
- 性别: GG
- 专业: 半导体光电子器件
3楼2015-12-01 09:58:22
4楼2015-12-01 10:46:33
zhuqw
金虫 (小有名气)
- 应助: 2 (幼儿园)
- 金币: 1217.4
- 帖子: 77
- 在线: 74.6小时
- 虫号: 2408038
- 注册: 2013-04-08
- 性别: GG
- 专业: 半导体光电子器件
5楼2015-12-01 14:26:54
shgao20
专家顾问 (职业作家)
-
专家经验: +809 - 仿真EPI: 1
- 应助: 1311 (讲师)
- 金币: 13381.4
- 红花: 267
- 帖子: 3531
- 在线: 473.4小时
- 虫号: 3644138
- 注册: 2015-01-14
- 专业: 动力学与控制
- 管辖: 仿真模拟
【答案】应助回帖
|
热分析时也要改为 solid90 - 20 节点六面体单元，在转换为结构分析时，会自动转换为 solid186 单元。 至于网格划分是否合理，有一份资料 "有限元网格划分的基本原则"，网上可以下载，你可以找来看看： http://wenku.baidu.com/view/a14dfe7102768e9951e73847.html?re=view http://wenku.baidu.com/view/ec36630abb68a98271feface.html?re=view |
6楼2015-12-02 08:19:38
7楼2016-11-06 23:50:51
8楼2017-11-23 16:16:39
