请教混凝土损伤塑性的收敛问题【已给出解决方法】

Analyst

这是一个关于桥梁极限承载力计算的问题。混凝土采用的是Concrete Damaged Plasticity模型。但是遇到了不收敛的问题。求助


1.结构组成
结构为中等跨度简支梁桥，跨度为30米， 所有模型都是由ansys导入生成的，实体单元选用C3D8R，都是较好的六面体单元，桥梁和墩子普通钢筋选用T3D2，预应力钢筋选用B31

模型信息如下：

1.桥梁

2.桥梁普通钢筋

3.墩子

4.墩子普通钢筋

5.预应力钢筋


钢筋混凝土采用组合式建模，普通钢筋和预应力钢筋embed到钢筋混凝土。


2.step和load部分共分为三个
第一部分为首先施加重力，第二步施加预应力到预应力钢筋（采用降温法），第三步为桥墩的沉降，目前的分析只有这三个部分

inp信息如下：

** STEP: gravity
**
*Step, name=gravity, nlgeom=YES, inc=1000000
*Static
0.0005, 0.1, 1e-10, 0.01
**
** LOADS
**
** Name: GRAVITY-1   Type: Gravity
*Dload
, GRAV, 9.8, 0., -1., 0.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-1
**
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
**
** STEP: yuyingli
**
*Step, name=yuyingli, nlgeom=YES, inc=1000000
*Static
0.0005, 0.1, 1e-10, 0.01
**
** PREDEFINED FIELDS
**
** Name: Field-1   Type: Temperature
*Temperature
YUYINGLISUO, 595.
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-2
**
*Output, field, variable=PRESELECT
**
** HISTORY OUTPUT: H-Output-2
**
*Output, history, variable=PRESELECT
*End Step
** ----------------------------------------------------------------
**
** STEP: setting
**
*Step, name=setting, nlgeom=YES, inc=1000000
*Static
0.0005, 0.1, 1e-10, 0.01
**
** BOUNDARY CONDITIONS

*****************
若干 BOUNDARY CONDITIONS信息
*****************

pbmcts

有意思回帖汇总：

11#
谢谢大家了，后来尝试了五方面的工作，顺利的收敛了——收敛了还要根据力学原理等判断计算结果是否可用。
第一是原先的模型网格画得很细，大约有60万节点的样子，一共有78万多单元，计算耗时很长，而且总是出现不收敛。后来将网格改粗了不少，节点变为20多万——有没再细化网格再算，网格粗细对结果还是有影响的。
第二个是改变了钢筋跟混凝土的接触方式。因为这是一个较为精细的模型，混凝土和钢筋分开建模，在最初的一些处理中，并没有用embed，而是合并节点的方式
。后来检查发现，改用了embed。
第三是混凝土的本构例如
*Concrete Damaged Plasticity
30.,    0.1,   1.16, 0.6667,     0
改为
*Concrete Damaged Plasticity
30.,    0.1,   1.16, 0.6667,     0..0005——粘性参数是依据什么取值的？
第四是把所有的step中的初始时间步改为0.0005
第五是本身是按照混凝土标准取得的本构值，再次按照帮助文档的方式进行了重新计算
收敛效果很明显。
14#
根据规范得到一组值，其中应变部分是总应变，包含了弹性应变，这个是需要去掉的
据别人经验，初始应力值取0.6的极限应力值——预应力筋取值？.
根据塑性应变=总应变-应力值/弹性模量得到塑性应变

16#
钢筋还是要用梁单元，很明显，模型中钢筋还是要承受弯矩的，桁架单元是不考虑弯矩影响，只考虑轴向方向的应力
17#
16# bearandyou truss单元通过力偶对提供弯矩抗力，使用beam单元无非多考虑钢筋截面自身的弯矩抗力，应该很小吧，而且beam单元embed在混凝土中，并不约束转动，意义不大？
19#
这里还是我疏忽了，没有看清楚，普通钢筋用的桁架单元，但是预应力钢筋还是用的梁单元，我看成桁架单元。
   一根钢筋抗弯能力比较小，甚至可以忽略，但是大量的钢筋时，就不能忽略混凝土中钢筋的抗弯能力了，具体问题具体对待。本例是高架桥问题，混凝土中钢筋不仅承受拉力还会提高混凝土抗弯能力，不可忽视其抗弯作用。
20#
19# bearandyou 还望讲得详细些，当用于混凝土结构（主抗弯）中时，二者的优势与劣势。预应力筋与普通筋的区别主要是什么呢？——采用什么单元模拟，是否考虑抗弯？如果使用梁单元的话，转动自由度如何处理呀？学习一下哈


25#
楼主的C40混凝土参数有问题，fc怎么可能达到39.6呢，你的C60才38左右
26#
我想问下，你预应力筋用的梁单元，截面是怎么定义的？比如说12.7的钢绞线，截面是圆形，你是把他面积换算成相应的直径建模的，还是直接用的12.7？
28#
嗯，粘性系数对收敛影响很大的
31#
但是弹性模型的取值该怎么办？是取初始弹性模量还是某一点的割线模量，在程序里面输入的弹性模型是不是初始弹性模型呢？对峰值应变和极限压应变有什么要求吗？期待解答。

Analyst

接着就是材料定义部分。这部分我尝试过四个混凝土本构
因为还是在试算阶段，我将钢筋设置为弹性材料，混凝土为损伤塑性。

第一个混凝土的本构是abaqus提供的。如下：

*Concrete Damaged Plasticity
15.,    0.1,   1.16, 0.6667,     0.
*Concrete Compression Hardening
  2.598e+07,     0.
3.1593e+07, 0.0004
3.4298e+07, 0.0008
    3.5e+07, 0.0012
3.4362e+07, 0.0016
3.2859e+07,  0.002
3.0835e+07, 0.0024
2.3696e+07, 0.0036
1.6113e+07,  0.005
  3.194e+06,   0.01
*Concrete Tension Stiffening
3.291e+06,     0.
2.693e+06, 0.0001
2.058e+06, 0.0003
1.775e+06, 0.0004
1.479e+06, 0.0005
   991000., 0.0008
   664000.,  0.001
   298000.,  0.002
   135000.,  0.003
    74000.,  0.005
第二种为 c50的本构，是一个网友提供的，数据不太方便发布

第三种是C40的本构

数据如下：

*Material,name=concrete
*Elastic
3.4e+04, 0.2
*Concrete Damaged Plasticity
30.,    0.1,   1.16, 0.6667,     0.!
*Concrete Compression Hardening
30,      0.
39.6,   0.0005
39.6,   0.001
15,      0.007
9,        0.02
*Concrete Tension Stiffening
3.5,     0.
1.2,     0.001
0.68,   0.01  

第四种为：
*MATERIAL, NAME=C60
*ELASTIC
3.60E10,0.3
*DENSITY
2500.
*CONCRETE DAMAGED PLASTICITY
35.,0.1,1.2,0.85,0.
*CONCRETE COMPRESSION HARDENING
10.80000E6,0.00000
21.24139E6,0.00030
28.84499E6,0.00060
30.90988E6,0.00070
32.73428E6,0.00080
34.31478E6,0.00090
35.64800E6,0.00100
36.73052E6,0.00110
37.55895E6,0.00120
38.12988E6,0.00130
38.43992E6,0.00140
38.48567E6,0.00150
38.12922E6,0.00160
37.43699E6,0.00170
36.48357E6,0.00180
35.34608E6,0.00190
34.09038E6,0.00200
32.76977E6,0.00210
31.42549E6,0.00220
30.08815E6,0.00230
28.77951E6,0.00240
27.51431E6,0.00250
26.30190E6,0.00260
25.14760E6,0.00270
24.05383E6,0.00280
23.02091E6,0.00290
22.04777E6,0.00300
21.13239E6,0.00310
16.69329E6,0.00370
12.06599E6,0.00470
9.322450E6,0.00570
7.548990E6,0.00670
6.322140E6,0.00770
5.428350E6,0.00870
4.750640E6,0.00970
4.220310E6,0.01070
3.794640E6,0.01170
3.445790E6,0.01270
3.154910E6,0.01370
2.908780E6,0.01470
2.697920E6,0.01570
2.515290E6,0.01670
2.355630E6,0.01770
2.214880E6,0.01870
2.089900E6,0.01970
*CONCRETE TENSION STIFFENING
0.36000E6,0.00000
0.59774E6,0.00001
0.89645E6,0.00002
1.19448E6,0.00003
1.49043E6,0.00004
1.78143E6,0.00005
2.06228E6,0.00006
2.32447E6,0.00007
2.55497E6,0.00008
2.73488E6,0.00009
2.83784E6,0.00010
2.81012E6,0.00011
2.65078E6,0.00012
2.45231E6,0.00013
2.25249E6,0.00014
2.06683E6,0.00015
1.90041E6,0.00016
1.75361E6,0.00017
1.62491E6,0.00018
1.51215E6,0.00019
1.41315E6,0.00020
1.32592E6,0.00021
1.24872E6,0.00022
1.18008E6,0.00023
1.11875E6,0.00024
1.06370E6,0.00025
1.01406E6,0.00026
0.96910E6,0.00027
0.92822E6,0.00028
0.89090E6,0.00029
0.64307E6,0.00039
0.51131E6,0.00049
0.42915E6,0.00059
0.37267E6,0.00069
0.33122E6,0.00079
0.29936E6,0.00089
0.27402E6,0.00099
0.25332E6,0.00109
0.23604E6,0.00119
0.22137E6,0.00129
0.20874E6,0.00139
0.19773E6,0.00149
0.18803E6,0.00159
0.17942E6,0.00169
0.17171E6,0.00179
0.16476E6,0.00189
0.15845E6,0.00199
*CONCRETE COMPRESSION DAMAGE, TENSION RECOVERY=1.
0.00000,0.00000
0.07707,0.00030
0.12437,0.00060
0.14008,0.00070
0.15625,0.00080
0.17290,0.00090
0.19006,0.00100
0.20776,0.00110
0.22604,0.00120
0.24494,0.00130
0.26451,0.00140
0.28481,0.00150
0.30712,0.00160
0.33082,0.00170
0.35532,0.00180
0.38004,0.00190
0.40453,0.00200
0.42847,0.00210
0.45162,0.00220
0.47384,0.00230
0.49503,0.00240
0.51515,0.00250
0.53420,0.00260
0.55219,0.00270
0.56916,0.00280
0.58515,0.00290
0.60021,0.00300
0.61440,0.00310
0.68403,0.00370
0.75973,0.00470
0.80720,0.00570
0.83938,0.00670
0.86250,0.00770
0.87988,0.00870
0.89339,0.00970
0.90420,0.01070
0.91302,0.01170
0.92037,0.01270
0.92658,0.01370
0.93189,0.01470
0.93649,0.01570
0.94051,0.01670
0.94405,0.01770
0.94719,0.01870
0.95000,0.01970
*CONCRETE TENSION DAMAGE
0.00000,0.00000
0.00001,0.00001
0.00010,0.00002
0.00044,0.00003
0.00133,0.00004
0.00331,0.00005
0.00717,0.00006
0.01402,0.00007
0.02541,0.00008
0.04342,0.00009
0.07093,0.00010
0.11484,0.00011
0.17402,0.00012
0.23445,0.00013
0.29118,0.00014
0.34258,0.00015
0.38842,0.00016
0.42907,0.00017
0.46508,0.00018
0.49704,0.00019
0.52550,0.00020
0.55095,0.00021
0.57379,0.00022
0.59440,0.00023
0.61306,0.00024
0.63002,0.00025
0.64551,0.00026
0.65970,0.00027
0.67275,0.00028
0.68479,0.00029
0.76807,0.00039
0.81503,0.00049
0.84530,0.00059
0.86654,0.00069
0.88230,0.00079
0.89451,0.00089
0.90425,0.00099
0.91222,0.00109
0.91888,0.00119
0.92452,0.00129
0.92937,0.00139
0.93359,0.00149
0.93729,0.00159
0.94058,0.00169
0.94351,0.00179
0.94614,0.00189
0.94851,0.00199

Analyst

上述四种材料本构不收敛停止计算的错误均为

too many attemps made for this increment

第一种材料本构在计算第一步的最初即出现迭代不成功的现象出现，错误类型不说了
第二种和第四种是在计算到step2的时候通不过
第三种材料本构在计算第三步通不过。

Analyst

关于第三种材料本构计算不收敛中 显示的警告如下：

For *tie pair (assembly_bridgenode_cns__cns__cns__cns_-assembly_dunzi), adjusted nodes with very small adjustments were not printed. Specify *preprint,model=yes for complete printout.
The option *temperature is used but the option *initial conditions,type=temperature is not. The initial temperature values are assumed to be zero.
312 elements are distorted. Either the interior angles are out of the suggested limits or the triangular or tetrahedral quality measure is bad. The elements have been identified in element set WarnElemDistorted.
For 2030 beam elements either the average curvature about the local 1-direction differs by more than 0.1 degrees per unit length as compared to the default curvature or the approximate integrated curvature for the entire beam differs by more than 5 degrees as compared to the approximate integrated default curvature. This may be due to a user-specified normal or due to the nodal averaging routine used by Abaqus. This difference may cause unexpected behavior of the beam and you may want to verify that the beam normals are correct for your problem. The elements have been identified in element set WarnBeamCurvature1.
For 680 beam elements either the average curvature about the beam tangent differs by more than 0.1 degrees per unit length as compared to the default curvature or the approximate integrated curvature for the entire beam differs by more than 5 degrees as compared to the approximate integrated default curvature. This may be due to a user-specified normal or due to the nodal averaging routine used by Abaqus. This difference may cause unexpected behavior of the beam and you may want to verify that the beam normals are correct for your problem. The elements have been identified in element set j_WarnBeamTwist.
Boundary conditions are specified on inactive dof of 882 nodes. The nodes have been identified in node set WarnNodeBCInactiveDof.
The system matrix has 4 negative eigenvalues.
The plasticity/creep/connector friction algorithm did not converge at 1 points
The system matrix has 6 negative eigenvalues.
The system matrix has 4 negative eigenvalues.
The system matrix has 4 negative eigenvalues.
The system matrix has 4 negative eigenvalues.
The system matrix has 4 negative eigenvalues.
The system matrix has 2 negative eigenvalues.
The plasticity/creep/connector friction algorithm did not converge at 1 points
The plasticity/creep/connector friction algorithm did not converge at 2 points
The system matrix has 2 negative eigenvalues.

Analyst

最后一步，即step3中的第六次收敛性检查信息如下：

CONVERGENCE CHECKS FOR EQUILIBRIUM ITERATION     6


AVERAGE FORCE                      1.664E+04   TIME AVG. FORCE       1.663E+04
LARGEST RESIDUAL FORCE              9.79       AT NODE      58005   DOF  1
   INSTANCE: BRIDGE-1-LIN-4-1                                                               
LARGEST INCREMENT OF DISP.         1.549E-08   AT NODE      58005   DOF  1
   INSTANCE: BRIDGE-1-LIN-4-1                                                               
LARGEST CORRECTION TO DISP.        1.730E-09   AT NODE      58005   DOF  1
   INSTANCE: BRIDGE-1-LIN-4-1                                                               
          DISP.    CORRECTION TOO LARGE COMPARED TO DISP.    INCREMENT

AVERAGE MOMENT                      64.7       TIME AVG. MOMENT       64.7   
LARGEST RESIDUAL MOMENT            0.162       AT NODE      39107   DOF  6
   INSTANCE: YUYINGLISUO-1-LIN-4-1                                                           
LARGEST INCREMENT OF ROTATION     -2.637E-07   AT NODE      39107   DOF  6
   INSTANCE: YUYINGLISUO-1-LIN-4-1                                                           
LARGEST CORRECTION TO ROTATION     3.577E-08   AT NODE      39107   DOF  6
   INSTANCE: YUYINGLISUO-1-LIN-4-1                                                           
          ROTATION CORRECTION TOO LARGE COMPARED TO ROTATION INCREMENT


***NOTE: THE SOLUTION APPEARS TO BE DIVERGING. CONVERGENCE IS JUDGED UNLIKELY.


***ERROR: TIME INCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED



     ANALYSIS SUMMARY:
     TOTAL OF         87  INCREMENTS
                      19  CUTBACKS IN AUTOMATIC INCREMENTATION
                     361  ITERATIONS INCLUDING CONTACT ITERATIONS IF PRESENT
                     361  PASSES THROUGH THE EQUATION SOLVER OF WHICH
                     348  INVOLVE MATRIX DECOMPOSITION, INCLUDING
                       0  DECOMPOSITION(S) OF THE MASS MATRIX
                       1  REORDERING OF EQUATIONS TO MINIMIZE WAVEFRONT
                       0  ADDITIONAL RESIDUAL EVALUATIONS FOR LINE SEARCHES
                       0  ADDITIONAL OPERATOR EVALUATIONS FOR LINE SEARCHES
                    2652  WARNING MESSAGES DURING USER INPUT PROCESSING
                      11  WARNING MESSAGES DURING ANALYSIS
                       0  ANALYSIS WARNINGS ARE NUMERICAL PROBLEM MESSAGES
                       8  ANALYSIS WARNINGS ARE NEGATIVE EIGENVALUE MESSAGES
                       1  ERROR MESSAGES



     JOB TIME SUMMARY
       USER TIME (SEC)      =   51730.   
       SYSTEM TIME (SEC)    =   449.40   
       TOTAL CPU TIME (SEC) =   52179.   
       WALLCLOCK TIME (SEC) =       7688

Analyst

由于INP有点大，上传不方便，见谅

shanhuimin923

312 elements are distorted. Either the interior angles are out of the suggested limits or the triangular or tetrahedral quality measure is bad. The elements have been identified in element set WarnElemDistorted.
For 2030 beam elements either the average ...... This may be due to a user-specified normal or due to the nodal averaging routine used by Abaqus. This difference may cause unexpected behavior of the beam and you may want to verify that the beam normals are correct for your problem. The elements have been identified in element set WarnBeamCurvature1.

Analyst 发表于 2010-6-23 10:32

从警告信息来看，你的问题不像是出现在材料本构这一块，应该是钢筋建模这一块问题比较大，不知你查看了 这两个红色的 set里面到底何指了没有？？

Analyst

7# shanhuimin923

这个我看到了，这个是因为预应力钢筋是空间曲线，所以出先orientation的方向不太一致，但是我这个是圆截面，应该不会造成这个问题吧！

wild_field

感觉模型建的很好，这种不收敛很有可能是由于软件本身计算能力达到大限，你不就是要计算极限载荷吗？而不是要计算桥梁坍塌的过程吧，所以计算到了极限停止后，也差不多就是极限承载力了。调整一些计算的参数可能使计算向前在算几步，以上是我瞎说的，仅供看看。

Analyst

9# wild_field

还没开始算极限状态

Analyst

谢谢大家了，后来尝试了五方面的工作，顺利的收敛了

第一是原先的模型网格画得很细，大约有60万节点的样子，一共有78万多单元，计算耗时很长，而且总是出现不收敛。后来将网格改粗了不少，节点变为20多万

第二个是改变了钢筋跟混凝土的接触方式。因为这是一个较为精细的模型，混凝土和钢筋分开建模，在最初的一些处理中，并没有用embed，而是合并节点的方式。后来检查发现，改用了embed。

第三是混凝土的本构例如
*Concrete Damaged Plasticity
30.,    0.1,   1.16, 0.6667,     0
改为
*Concrete Damaged Plasticity
30.,    0.1,   1.16, 0.6667,     0..0005

第四是把所有的step中的初始时间步改为0.0005

第五是本身是按照混凝土标准取得的本构值，再次按照帮助文档的方式进行了重新计算
收敛效果很明显。

junhuahuo.love

先收藏了，慢慢研究一下，多谢！

liyangshark

这位大哥能讲讲你的混凝土本构，Concrete Compression Hardening 之类的是如何换算的吗？怎么从混凝土的应力应变关系换算成aba中输入的参数？ 11# Analyst

Analyst

13# liyangshark
根据规范得到一组值，其中应变部分是总应变，包含了弹性应变，这个是需要去掉的
据别人经验，初始应力值取0.6的极限应力值.
根据塑性应变=总应变-应力值/弹性模量得到塑性应变

nuanshuipingbb

学习了。。。。

bearandyou

钢筋还是要用梁单元，很明显，模型中钢筋还是要承受弯矩的，桁架单元是不考虑弯矩影响，只考虑轴向方向的应力

jaylin628

16# bearandyou truss单元通过力偶对提供弯矩抗力，使用beam单元无非多考虑钢筋截面自身的弯矩抗力，应该很小吧，而且beam单元embed在混凝土中，并不约束转动，意义不大？

kid0317

学习了，钢筋自身的抗弯效果可能并不大

bearandyou

这里还是我疏忽了，没有看清楚，普通钢筋用的桁架单元，但是预应力钢筋还是用的梁单元，我看成桁架单元。
   一根钢筋抗弯能力比较小，甚至可以忽略，但是大量的钢筋时，就不能忽略混凝土中钢筋的抗弯能力了，具体问题具体对待。本例是高架桥问题，混凝土中钢筋不仅承受拉力还会提高混凝土抗弯能力，不可忽视其抗弯作用。

jaylin628

19# bearandyou 还望讲得详细些，当用于混凝土结构（主抗弯）中时，二者的优势与劣势。预应力筋与普通筋的区别主要是什么呢？如果使用梁单元的话，转动自由度如何处理呀？学习一下哈