Reduced integration scheme in the case of nonlinear analysis

tonnyw

This is one of the benchmark problems that Bathe employed to illustrate the problem that could happen in the case of nonlinear analysis for reduced integration scheme.
Can someone use Abaqus to run the model with both full integration and reduced integration to see how different the results are?

Your help is appreciated.

zsq-w

确认下：
1）lz想比较哪些结果？最大应力还是方块最大位移？Or both？ 建模的时候能不能忽略那2个truss？
2）图中数据是不是指：
E=2E12  yield=1GPa   F=5kN?

tonnyw

确认下：
1）lz想比较哪些结果？最大应力还是方块最大位移？Or both？ 建模的时候能不能忽略那2个truss？
>Sorry for not making it clear. I should mention that the analysis should be material nonlinearity only. Tangent modulus is zero. The output should be the plot of the force F versus its displacement along X axis. The two truss elements cannot be neglected.
According to Bathe, if we use reduced integration, we can see that the plane stress element collapses once the truss elements reach plasticity.

2）图中数据是不是指：
E=2E12  yield=1GPa   F=5kN?
zsq-w 发表于 2011-2-20 13:05

>The unit is okay since it is consistent for all the parameters. It may not make sense in reality though.

Also there are some glitches in the plot and the fix is attached.

The two truss elements have length of 10 while the length and height of the rectangle are 10 and 1 respectively.

zsq-w

好，哪位用abaqus做出来，我来加积分。

rocky11

中间平面应力单元是不是缺少几何信息？宽度是1，长度是2？
能不能解释一下可能出现的问题是什么呢？

rocky11

刚接触有限元理论，也没有完全理解lz的问题，所以只做了弹性的完全积分，缩减积分没调收敛，不知道这是不是问题所关注的？上个inp，期待高手解答和lz的结论

tonnyw

刚接触有限元理论，也没有完全理解lz的问题，所以只做了弹性的完全积分，缩减积分没调收敛，不知道这是不是问题所关注的？上个inp，期待高手解答和lz的结论
rocky11 发表于 2011-2-21 09:31

I think the results you have are correct. I ran the same model in Adina and got the similar results for elastic-only analysis. For elastic-plastic analysis, the model collapses even for full integration when the material yields. So there is an error in the original model saying that full integration works okay for elastic-plastic analysis while reduced integration not.

The reason that reduced integration is not working is that in this case the spurious zero energy mode in the eight-noded plane stress element is made free and the stiffness matrix is singular.

If you check the rank of the stiffness matrix for plane stress element, you can see that the rank is 13 for full integration and 12 for reduced integration. The missing rank corresponds to the spurious zero energy mode.

JingheSu

7# tonnyw Does abaqus have the ability to output the  Rank of stiffness matrix directly?

JingheSu

7# tonnyw Does abaqus have the ability to output the  Rank of stiffness matrix directly?

tonnyw

7# tonnyw  Does abaqus have the ability to output the  Rank of stiffness matrix directly?
JingheSu 发表于 2011-2-22 09:55

No. I don't think so. I output the element stiffness matrix and calculate its rank using Maple.