Abaqus错误与警告信息汇总(适合初学者)(转载内容)

ABAQUS模拟出现问题,都需要去monitor,msg文件中查看原因,如何分析这些信息呢?这个需要具体问题具体分析。不收敛的问题千奇万状,大致需要从接触、单元类型、边界条件、网格质量以及它们的组合等出着手。一般类似于:

 1)Fixed time is too large; 

2)Too many attamps have been made; 

3)THE SOLUTION APPEARS TO BE DIVERGING; 

4)CONVERGENCE ISJUDGED UNLIKELY;

 5)Time increment required is less than the minimum specified。 

这样的信息除了告诉你的模型分析失败以外,没有告诉你任何有用的东西,几乎是无用信息。需再查找别的信息来考察。 一般从模型的设置入手,必须说明的是:Error和warning的性质是完全不同的。Error意味着运算失败,但是出现warning可能还能算,而且有些运算必定会出现warning(比如接触分析必定出“负特征值”,下有详述)。

很多警告只是通知性质的,或者只是说明一下而已,不一定都是模型有问题。比如以下warning完全可以忽略: 1) xxxxx will (not) printed;这种只是通知你一声,某些东西不输出了。 2)The parameter frequency cannot be used with the parameter field. It will be ignored;都说某某被ignored了。

 先分类做一下介绍: 

(一)

如果模型能算,且结果合理,那么大部分警告信息可以不管。但是以下除外:

1)numerical sigularity(数值奇异)、刚体位移(欠约束)solver problem;numerical sigularity when processing node105 instance pile D.O.F. 1 ratio=1.735e13 

2)Zero pivot(零主元);过约束或者欠约束。 

这两个问题一般都意味着模型约束存在问题。问题1)、2)都会伴随着产生大量负特征值,解决方案当然是检查约束。 

(二)

有一些直接导致计算aborted,那就得仔细分析了,比如: 

1)xxxxx is not a valid in ABAQUS/Standard;告诉你这种计算standard不支持了,换别的。

 2)missing property;在perperty步检查材料属性是不是都加上了。如果有梁单元,看看梁法向定义对了没有。 

3)Detected lock file Job-1.lck. Please confirm that no other applications are attempting to write to the output database associated with this job before removing the lock file and resubmitting;删除.lck文件就可以了,它是一个自动生成的文件。你也可以另存为(另取名),再运算。

4)The rigid part xx is missing a refernce point;刚体(or刚体约束)都必须通过stools--reference point给它定义一个参考点(RP),载荷都加在这个RP上。 

5)The area of 54 elements is zero,small,or negative.Check coordinates or node numbering,or modify the mesh seed.The elements 8 have been identified in element set ErrElemAreaSmallNegZero;这个一般是节点编号不对的问题。必须是逆时针方向。 

6)The value of 256 MB that has been specified for standard_memory is too small to run the analysis and must be increased. The minimum possible value for standard_memory is 470 MB 

7)HM to ABA的问题:集合和面的几何的名称最好不要用特殊符号和数值,全部用英文字母是最安全的。 

8)令很多人抓狂的error code 5 

a)使用了子程序, 子程序有问题。 

b)模型有问题, 通常模型很大,很复杂。 

Please make sure that the mesh density of the slave surface in the tie pair is finer than the master surface. The analysis may run slower, may yield inaccurate results, and may require more memory if this is not the case 

c)硬盘没空间了(这个其实不会引起error code 5,但是出错是肯定的了), 或者是内存太小.或者产生的文件太大。 

d)关闭杀毒软件试试(特别是卡巴)。 

e)有人认为边界条件不正确,也会引起这个错误. 

9)system error code 29539 ;关闭杀毒软件and try。 

10)**ERROR: Issue cannot be deleted Not all data Released;在windows中,单击“控制面板”--“系统”--“高级”--“性能设置”--“数据执行保护”命令,把pre.exe和standard.exe添加进去。重起动后尝试。 

11)Surfaces associated with analytical rigid part MANDREL may have their orientation flipped刚体相连的接触面方向定义反了,在接触定义的地方edit--flip 

12)CONTACT PAIR (ASSEMBLY_BLANKBOT,ASSEMBLY_TIE-1_DIEDURF) NODE BLANK-1.5 IS OVERCLOSED BY 0.0512228 WHICH IS TOO SEVERE;这往往是因为接触面的法线方向定义反了。定义刚体和shell的surface时,要注意选择外侧。 

13)123456 elements are distorted。Excessive distortion of element number 5 of instance PART-1-1;如果有子程序,一般不是材料设置有问题,就是边界条件的问题。 

14)XML parsing failure for job 1.Shutting down socket and terminating all further messages.Please check the .log, .dat, .sta, or .msg files for information about the status of the job. 

15)The number of history output requests in this ABAQUS analysis (>5000)may cause SIGNIFICANT performance problems during analysis and postprocessing;输出项太多,恐硬件资源不够。要是你确保硬件够,这条也不怕了。一般的,应该减少History中的输出项,尽量输出你最感兴趣的内容。 

16)Value for parameter nset will be truncated to 80 characters;nset名字取太长了,80字符限制。

17)compilation - ifort.exe。Problem during compilation - ifort.exe not found in PATH;安装的时候没有装好或是二次开发版本冲突。检查环境变量的设置;然后verify一下,看看是子程序功能否能通过。 

(三)

如上所说,有很多warning并一定意味着你的模型存在问题。常被问起的有: 

1)负特征值问题r> THE SYSTEM MATRIX HAS 8 NEGATIVE EIGENVALUES;负特征值是非线性分析的必然产物。所以不必大惊小怪,甚至久而久之,对于你熟悉的问题,你都会视而不见了。若出了问题,可先检查下有没有伴随的numerical sigularity(数值奇异)和Zero pivot(零主元)产生。如果没有,可以参考这几个方面: 

a)刚体位移; 

b)单元异常,过度变形、过度扭曲等; 

c)应力应变关系有负斜率 

d)如果有流体的话,在容器发生形变的话,也可能出现negative eigenvalue的情况,不过不会出现警告,这是被允许的; 

e)失稳发生。 

2)The ratio of deformation speed to wave speed exceeds 1.0000;这个警告是指单元形变速度V(单元最大形变率/特征尺寸)和膨胀波速C(通过材料本构关系求得)的比例超过1,解决这个问题的方案有以下几种: 

a)检查单位是否封闭(参数设置有数量级的错误),此错误新手常犯; 

b) 检查网格质量; 

c) 检查加载速度,如果条件允许的话就降低速度,该方法也很有效,但在很多情况下无法降低速度; 

d) 调整STEP中的TIME SCALING FACTOR;调整STEP MASS SCALING FACTOR; 

e) 加*SECTION CONTROLS,NAME=SC,DISTORTION CONTROL,LENGTH RATION=0.1或者YES也可以,加在MATERIAL 前面;或加* DIAGNOSTICS,DEFORMATION SPEED CHECK=OFF;或者加*DIAGNOSTICS, CUTOFF RATIO=RATIO(具体数值),在其他方法修改后还有问题的的情况下使用增加 

3)force/ZERO MOMENT问题 THERE IS ZERO MOMENT EVERYWHERE IN THE MODEL BASED ON THE DEFAULT CRITERION. PLEASE CHECK THE VALUE OF THE AVERAGE MOMENT DURING THE CURRENT ITERATION TO VERIFY THAT THE MOMENT IS SMALL ENOUGH TO BE TREATED AS ZERO. IF NOT, PLEASE USE THE SOLUTION CONTROLS TO RESET THE CRITERION FOR ZERO MOMENT;这个警告是告诉你模型中没有弯矩,没问题的,可以继续计算。如果提示中出现特征值奇异的时候才是计算有可能出现不收敛的问题。 

4)Degree of freedom 4 is not active in this model and can not be restrained;有限元软件计算对于实体步考虑转动自由度,所以你在边界条件中限制了456的自由度后,软件会忽略的啊。 

5)The option *boundary,type=displacement has been used;check status file between steps for warnings on any jumps prescribed across the steps in displacement values of translational dof. For rotational dof make sure that there are no such jumps.All jumps in displacements across steps are ignored;你采用了位移边界条件,但在平动自由度上,可能在不同的分析步骤里面有突变(你可以从sta文件里面查看),并且应保证转动自由度无突变。通知性质的warning,一般是因为你采用位移加载方式,都出这个。 

6)The strain increment has exceeded fifty times the strain to cause first yield at 377 points;检查下约束够不够,约束够了就不用管了,这只是通知你,你的模型塑性应变很大,一般没多大问题。 

7)123 nodes are used more than once as a slave node in *TIE keyword.One of the *TIE constraints at each of these nodes have been identified in node set WarNodeOverconTieSlave;定义接触的时候,公共节点重复定义了好几次,这样可能会出现过约束问题(只是可能影响) 

8)There are 2 unconnected regions in the model;可能是接触面有空隙,最好在接触属性中定义一个容差范围。一般各个parts之间定义接触,aba都会这样通知用户的,只要接触设置对了,一般没事。 

9)Boundary conditions are specified on inactive dof of 124 nodes.The nodes have been identified in node set WarnNodeBCIactiveDof;边界条件定义的有问题:在124个节点的非自由度上有边界加载。 

10)The plasticity/creep/connector friction algorithm did not converg;一般是塑性应变太大,单元扭曲导致的。可以先改为弹性模型看看是否收敛。 

11)The ratio of the maximum incremental adjustment to the average characteristic length is 1.82846e-02 at node 10868 instance jiti1 on the surface pair (assembly_jq22,assembly_q22);可以通过调大预设值消除该提示并检查网格质量。 

12)ELEMENT 42 INSTANCE SOIL3-1 IS DISTORTING SO MUCH THAT IT TURNS;应改进单元质量。 

13)650 nodes are either missing intersection with their respective master surface or outside the adjust zone;改改tie里的tolarance试试。 

14)Dependent part instances cannot be edited or assigned mesh attributes;模型树--assembly-打击part 右键--make independent。也可以到模型树part步展开点mesh。 

15)The aspet ratio for nnn elements exceeds 100 to 1;单元划分网格长宽比不合适。如果这些单元在不重要的区域(对结果肯定有些影响,影响大小取决于这三个单元的位置,在模型中的作用等),而且能计算,那就没问题了。 

16)123 elements are distorted;存在单元扭曲,如果这些单元在不重要的区域(对结果肯定有些影响,影响大小取决于这三个单元的位置,在模型中的作用等),而且能计算,那就没问题了。 

17)***WARNING: DEGREE OF FREEDOM 1 IS NOT ACTIVE ON NODE 6 - THIS BOUNDARY CONDITION IS IGNORED;约束了单元没有的自由度对求解没有影响,可以查看下。 

18) 热分析时出现了这样的警告“THERE IS ZERO HEAT FLUX EVERYWHERE There is zero HEAT FLUX everywhere in the model based on the default criterion. please check the value of the average HEAT FLUX during the current iteration to verify that the HEAT FLUX is small enough to be treated as zero.if not, please use the solution controls to reset the criterion for zero HEAT FLUX.

试试: (1)是不是热源定义的问题,错误信息是说热源量几乎为零。 (2)定义热源的子程序调用命令流应该为*HEAT GENERATION,在材料模块中定义,子程序为HETVAL。 

19) The elements in the element set WarnElemSurfaceIntersect-Step1 are involved surface intersections. Refer to the status and message file for further details;检查一下你单元集合的定义以及面的定义,看是否出现了相交或重复定义的情况。 

20)Boundary conditions are specified on inactive dof of 36 nodes. The nodes have been identified in node setWarnNodeBCInactiveDof. 

21)Integration and section point output variables will not be output for deformable elements that are declared as rigid using the *rigid body option;这个仅是通知性质的(在interaction步设置为rigid body,不输出应力应变),你在interaction步定义了刚体约束的话,都会出这个警告。 

22)For a self contact surface, the facets of the elements in element set WarnElemFacetThick Pt63d-Step1 are thicker than 0.6 times an edge or diagonal length of the facets. Use the MAXRATIO parameter on *SURFACE DEFINITION to allow automatic rescaling of the contact thicknesses where necessary for this surface.Refer to the status file for further details. 

23)NO VALID RADIATION OUTPUT REQUESTS HAVE BEEN GENERATED. THIS MAY BE DUE TO EARLIER INPUT ERRORS OR SPECIFICATION OF A NONEXISTANT CAVITY OR SURFACE NAME;检查一下你的output設定裡是不是有些set或surface沒有設定到。 

24)123 nodes may have incorrect normal definitions. The nodes have been identified in node set WarnNodeIncorrectNormal;先用看看WarnNodeIncorrectNormal在哪儿。这个不一定是致命的警告,有时候可以忽略。如果模型不收敛,可以检查下是否有过约束,在接触上存在边界条件or加载。 

(四)

比较有价值的的信息考察。比如: 

1)Numerical sigularity solver problem. numerical sigularity when processing node105 instance 表示:数值奇异:刚体位移(欠约束) 

2)Zero pivot 表示:过约束 

3)对于TIME INCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED,Too many attamps have been made 

4)对于“网格扭曲”的警告: excessively distorted elements 前面有提到。

 第一步:采用display查看“ ErrElemExcessDistortion-Step1 ”在模型的哪些部位,做到心中有数。 

第二步:检查模型的网格质量: mesh步---verify----Analysis Check选取模型。这种情况,一开始计算即出现“distorted element”的信息。除此之外,很多其他问题也会网格扭曲警告。比如,几何模型导入有误需要修补、单元类型选取错误、边界条件有误、材料属性错误、接触设置不合理、子程序错误等。

 第三步:即使你的网格划分很好,如果变形过大,也会导致网格扭曲。然后修改网格划分,不要出现红色,关键区域不要出现黄色。(当然最好是所有的网格都用structure划分,且都没有红色、黄色出现。网格质量就比较好。这种情况,警告信息往往是在计算到一定步骤之后才出现“distorted element”。 这种情况建议采用ALE等方式。

ABAQUS错误警告

Abaqus错误与警告信息汇总(适合初学者)(转载内容)的评论10条

  • Hs小毕
    0
    补充一个Connections is error.这个一般来说断网计算就不出现了。
  • 李焱鑫
    0
    节点过度旋转怎么破

Abaqus错误与警告信息汇总(适合初学者)(转载内容)的相关案例教程

status文件如下 ------------------------------------------------------------------------------- PREPROCESSOR WARNING MESSAGES -------------------------------------------------------------------------------
Too many attempts made for this increment The analysis has been terminated due to previous errors. All output requests have been written for the last converged increment. Abaqus/Standard Analysis exit
Whenever a translation (rotation) dof at a node is constrained by a kinematic coupling definition the translation (rotation) dofs for that node cannot be included in any other constraint including mpc
Beginning of keyword reader 05/10/22 12:18:29 Memory required to process keyword : 19091970 *** Warning 20282 (STR+282) warpage angle of element ID= 2366 is computed as 1.6715E+02 degrees. *** Warning
三.AWS ParallelCluster 4. Workflow to create Linux cluster on AWS (4) Modify AWS ParallelCluster configuration file for creating Linux cluster •Go to console of EC2 instance: amazonlinux ▪Edit cluster
本科/CAE工程师
影响力
粉丝
内容
获赞
收藏
    项目客服
    培训客服
    10 44