【讨论】请教大侠们一个关于：Large Deformation 的问题。

hohct

偶在两个刚体(RIGID SURFACE)平面之间压一个圆环(CPE4)，MSG 总是出现：  
***WARNING: THE STRAIN INCREMENT HAS EXCEEDED FIFTY TIMES THE STRAIN TO CAUSE  
             FIRST YIELD AT 460 POINTS
  
  ***WARNING: THE STRAIN INCREMENT IS SO LARGE THAT THE PROGRAM WILL NOT ATTEMPT  
             THE PLASTICITY CALCULATION AT 364 POINTS
  
  ***WARNING: CONVERGENCE JUDGED UNLIKELY.  INCREMENT WILL BE ATTEMPTED AGAIN  
             WITH A TIME INCREMENT OF 9.76563E-14
  
那位大侠有高见， 不甚感激！！！
hohct2000@hotmail.com

silt

不一定是大变形或大应变问题。根据我的经验，可能是你在某些分析步（step）中所施加的作用（如荷载）过大。适当减小看还是否出这类警告？
祝好运。

lxuejin

我也遇到过这个问题，是不是某些区域进入了严重的塑性？
请高人解释一下

jjjpark18

I got the following information from "ABAQUS Answers" at www.abaqus.com, it may give you some hints.
  
---------------------------------------------------------------------------------------------------
  Question  
  In the message file of my analysis there are warnings that the current strain increment exceeds the strain to first yield by more than 50 times; what does this mean?
   
   
  Answer  
  (The following applies to all versions.)
  
This warning message is issued only if something in the model is causing relatively large deformations in a problem in which the material model is some form of plasticity.
  
The causes may be erroneous input data, poor meshes, or instabilities developing in the model after some deformation.  
  
// Does the message occur in the first increment? If so, the input data are probably incorrect. Check the following:
  
- Is the loading excessive?  
- Is the magnitude of loading physically realistic?  
- Are the units correct with respect to the rest of the model?  
- If this is a dynamic analysis, are the units for density correct?  
  
// If the message occurs after some plastic deformation has developed:  
  
- Check the stress-plastic strain data. Make sure the material data do not become perfectly plastic at too low a plastic strain. If they do, add a small amount of hardening up to very large plastic strains. If you need to have the material go perfectly plastic, it may be necessary to use *STATIC, RIKS. See "Unstable collapse and post-buckling analysis," Section 6.2.4 of the Version 6.2 or Version 6.3 ABAQUS/Standard User's Manual.  
  
- Is the mesh refinement adequate? Meshes that are adequate for linear elasticity may not be adequate for large-strain plasticity problems. If the elements for which this message is being given are in a region where the geometry changes rapidly, the mesh in this region may need to be refined.  
  
- If neither of the above problems is the cause, the message may be due to unstable deformation (possibly local). Look at the increments just prior to the occurrence of the problem and see if a physical instability seems reasonable. The STABILIZE parameter on the *STATIC, *COUPLED TEMPERATURE-DISPLACEMENT, *SOILS, or *VISCO options may stabilize the model sufficiently so that this problem does not occur. See "Solving Nonlinear Problems," Section 8.2.1 of the Version 6.2 or Version 6.3 ABAQUS/Standard User's Manual, and "Unstable collapse and postbuckling analysis," Section 6.2.4 of the Version 6.2 or Version 6.3 ABAQUS/Standard User's Manual.