壳单元与实体单元接触分析怎么定义接触？
壳单元建立模型是在中面建立的，可接触面不是中面，如何定义接触对 壳单元和实体单元间有一定的空隙，为壳单元厚度的一般，在打开eshape时能够接触，然后在接触单元174中设置keypot(11)为include，表示包含壳厚度的影响 多谢。shell181和solid45可以用接触分析吗 。shell181和solid45定义接触分析出现*** WARNING *** CP = 402.547 TIME= 22:01:29
All selected contact pairs are initially open.Rigid body motion can
occur.You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps.
*** WARNING *** CP = 402.734 TIME= 22:01:29
The only selected contact pair is initially open.Rigid body motion
may occur in any portion of the model held in place solely by contact
elements.
回复 #3 jsp613 的帖子
shell181和solid是可以用接触分析的，出现的警告，第一个没什么问题，只要你打开了壳单元的厚度效应。第二警告出现的原因应该不是由单元选择引起的 You may use auto CNOF/ICONT by setting KEYOPT(5) to close small gaps.能具体讲讲auto CNOF/ICONT吗 ？setting KEYOPT(5) to close small gaps.没找到这个close small gaps选项，只有
KEYOPT(5)
CNOF/ICONT Automated adjustment:
0 --
No automated adjustment
1 --
Close gap with auto CNOF
2 --
Reduce penetration with auto CNOF
3 --
Close gap/reduce penetration with auto CNOF
4 --
Auto ICONT 我打开了壳单元厚度效应的，定义接触对后弹出第一个警告
All selected contact pairs are initially open.Rigid body motion can
occur.You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps.
把KEYOPT(5)设为1可以吗？没看到 close small gaps.什么原因呢第一个警告
check接触对时出现第二个警告The only selected contact pair is initially open.Rigid body motion
may occur in any portion of the model held in place solely by contact
elements. 这个警告又是什么原因？要紧吗？再次麻烦斑竹 请版主再看看。 check接触对时提示：
*** NOTE *** CP = 96.984 TIME= 09:24:55
Deformable-deformable contact pair identified by real constant set 3
and contact element type 4 has been set up.
Contact algorithm: Augmented Lagrange method
Contact detection at: Gauss integration point
Beam/shell thickness effect is included.
Contact stiffness factor FKN 1.0000
The resulting contact stiffness 0.12984E+10
Penetration tolerance factor FTOLN 0.10000
The resulting penetration tolerance 0.20000E-03
Max. initial friction coefficient MU 0.10000
Default tangent stiffness factor FKT 1.0000
Default elastic slip factor SLTOL 0.10000E-01
The resulting elastic slip 0.99981E-05
Update contact stiffness for each sub-load step
Max. friction stress TAUMAX 0.10000E+21
Average contact surface length 0.99981E-03
Average contact pair depth 0.20000E-02
Default pinball region factor PINB 1.0000
The resulting pinball region 0.20000E-02
Auto contact offset used to close gap 0.0000
*WARNING*: Initial penetration is included.
*** NOTE *** CP = 96.984 TIME= 09:24:55
No contact was detected for this contact pair.
****************************************
*** WARNING *** CP = 96.984 TIME= 09:24:55
All selected contact pairs are initially open.Rigid body motion can
occur.You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps.
1 CONTACT PAIR IS SELECTED
CONTACT PAIR HAVING REAL ID = 3 IS INITIALLY OPEN
BUT MAY BE AUTOMATICALLY CLOSED
err文件中提示：
*** WARNING *** CP = 78.859 TIME= 09:22:53
The only selected contact pair is initially open.Rigid body motion
may occur in any portion of the model held in place solely by contact
elements.
*** WARNING *** CP = 96.984 TIME= 09:24:55
All selected contact pairs are initially open.Rigid body motion can
occur.You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps. All selected contact pairs are initially open. Rigid body motion can occur. You may use auto CNOF/ICONT by setting KEYOPT(5) to close small gaps.请问这个警告提示，该如何处理啊？ 同求 关注中 lmmcnn 发表于 2009-5-27 21:19 static/image/common/back.gif
All selected contact pairs are initially open. Rigid body motion can occur. You may use auto CNOF/IC ...
接触面之间存在一定的初始间隙，在发生接触之前，有部分结构由于没有约束，会发生刚体位
可以根据你的具体情况尝试下面的集中方法：
1. 调整模型，尽量避免这种初始间隙的存在，可以适当存在微小的初始过盈
2. 建立若弱弹簧单元约束刚体位移
3. 接触建立之前约束自由的那部分结构，接触建立后再去掉该位移约束
这个第三条，比较难做到吧？
页:
[1]