Abaqus錯(cuò)誤與警告信息匯總

2016-11-24 by:CAE仿真在線來(lái)源:互聯(lián)網(wǎng)

模型不能算或不收斂,都需要去monitor,msg文件查看原因,如何分析這些信息呢?這個(gè)需要具體問(wèn)題具體分析,但是也存在一些共性。這里只是嘗試做一個(gè)一般性的大概的總結(jié)。如果你看見(jiàn)此貼就認(rèn)為你的warning以為迎刃而解了,那恐怕令你失望了。不收斂的問(wèn)題千奇萬(wàn)狀,往往需要頭疼醫(yī)腳。接觸、單元類型、邊界條件、網(wǎng)格質(zhì)量以及它們的組合能產(chǎn)生許多千奇百怪的警告信息。企圖憑一個(gè)警告信息就知道問(wèn)題所在,那就只有神仙有這個(gè)本事了。一個(gè)warning出現(xiàn)十次能有一回參考這個(gè)匯總而得到解決了,我們就頗為欣慰了。

類似于:

Fixedtime is too large

Toomany attamps have been made

THESOLUTION APPEARS TO BE DIVERGING.

CONVERGENCEISJUDGED UNLIKELY.

Timeincrement required is less than the minimum specified

這樣的信息幾乎是無(wú)用信息(除了告訴你的模型分析失敗以外,沒(méi)有告訴你任何有用的東西)。宜再查找別的信息來(lái)考察。根據(jù)經(jīng)驗(yàn),改小增量步也不一定能收斂,雖然也有人報(bào)告過(guò)改好的先例,我是從來(lái)沒(méi)有遇到過(guò),也從來(lái)沒(méi)有那個(gè)奢望。所以我一般從模型的設(shè)置入手。

必須說(shuō)明的是:Error和warning的性質(zhì)是完全不同的。Error意味著運(yùn)算失敗,but出現(xiàn)warning可能還能算,而且有些運(yùn)算必定會(huì)出現(xiàn)warning(比如接觸分析必定出“負(fù)特征值”,下有詳述)。很多警告只是通知性質(zhì)的,或者只是說(shuō)明一下而已,不一定都是模型有問(wèn)題。比如以下warning完全可以忽略:

xxxxx will (not) printed,這種只是通知你一聲,某些玩意兒不輸出了。還有:

The parameterfrequency cannot be used with the parameter field. It will be ignored(都說(shuō)某某被ignored了).

A系列

如果模型能算,且結(jié)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(數(shù)值奇異):剛體位移(欠約束)

solverproblem. numerical sigularity when processing node105 instance

pileD.O.F. 1 ratio=1.735e13

2 Zero pivot(零主元): 過(guò)約束或者欠約束。

這2個(gè)問(wèn)題一般都意味著模型約束存在問(wèn)題。1)、2)都會(huì)伴隨著產(chǎn)生大量負(fù)特征值。解決方案當(dāng)然第一步是檢查約束了。

B系列

有一些直接導(dǎo)致計(jì)算aborted,那就得仔細(xì)分析了,比如:

1 xxxxx is not avalid in ABAQUS/Standard(告訴你這種計(jì)算standard不支持了,換別的)

2 missing property

在perperty步檢查材料屬性是不是都加上了。如果有梁?jiǎn)卧?看看梁法向定義對(duì)了沒(méi)有。

3 Detected lockfile Job-1.lck. Please confirm that no other applications are attempting towrite to the output database associated with

thisjob before removing the lock file and resubmitting.

刪除.lck文件就可以了,它是一個(gè)自動(dòng)生成的文件。你也可以另存為(另取名),再運(yùn)算。

4 The rigid part xxis missing a refernce point

剛體(or剛體約束)都必須通過(guò)stools--reference point給它定義一個(gè)參考點(diǎn)(RP),載荷都加在這個(gè)RP上。

5 The area of 54elements is zero, small, or negative. Check coordinates or node numbering, ormodify the mesh seed.

Theelements 8 have been identified in element set ErrElemAreaSmallNegZero

這個(gè)一般是節(jié)點(diǎn)編號(hào)不對(duì)的問(wèn)題。必須是逆時(shí)針?lè)较颉?/span>

6 The value of 256MB that has been specified for standard_memory is too small to run the analysisand must be increased. The

minimumpossible value for standard_memory is 470 MB

7 HM to ABA的問(wèn)題:集合和面的幾何的名稱最好不要用特殊符號(hào)和數(shù)值(特別是從hm轉(zhuǎn)過(guò)來(lái)),全部用英文字母是最安全的。

8 令很多人抓狂的error code 5

1)使用了子程序, 子程序有問(wèn)題, (例如數(shù)組定義跟實(shí)際賦值不一致,這個(gè)我也遇到過(guò))

2)模型有問(wèn)題, 通常模型很大,很復(fù)雜(這個(gè)我沒(méi)遇到過(guò))

Pleasemake sure that the mesh density of the slave surface in the tie

pair(mbly__pickedset37_cns_,assembly__pickedsurf36) is finer than the mastersurface.

Theanalysis may run slower, may yield inaccurate results, and may require morememory if this is not the case

3)硬盤(pán)沒(méi)空間了(這個(gè)其實(shí)不會(huì)引起error code 5,但是出錯(cuò)是肯定的了), 或者是內(nèi)存太小.或者產(chǎn)生的文件太大.

4)關(guān)閉殺毒軟件試試(特別是卡巴)

5) 有人認(rèn)為邊界條件不正確,也會(huì)引起這個(gè)錯(cuò)誤.

9 systemerror code 29539

關(guān)閉殺毒軟件and try。

10 **ERROR: Issuecannot be deleted Not all data Released

在windows中,單擊“控制面板”--“系統(tǒng)”--“高級(jí)”--

“性能設(shè)置”--“數(shù)據(jù)執(zhí)行保護(hù)”命令,

把pre.exe和standard.exe添加進(jìn)去。重起動(dòng)后嘗試

11 Surfacesassociated with analytical rigid part MANDREL may have their orientationflipped

剛體相連的接觸面方向定義反了,在接觸定義的地方edit--flip

12 CONTACT PAIR(ASSEMBLY_BLANKBOT,ASSEMBLY_TIE-1_DIEDURF)

NODEBLANK-1.5 IS OVERCLOSED

BY0.0512228 WHICH IS TOO SEVERE

這往往是因?yàn)榻佑|面的法線方向定義反了。定義剛體和shell的surface時(shí), 要注意選擇外側(cè)

13 123456elements are distorted。Excessive distortion of element number 5 of instance PART-1-1

如果有子程序,一般不是材料設(shè)置有問(wèn)題,就是邊界條件的問(wèn)題

14 XML parsing failure for job 1. Shutting down socket and terminating all further messages. Pleasecheck

the.log, .dat, .sta, or .msg files for information about the status of the job.

http://forum.simwe.com/viewthrea... 26amp;typeid=68

15 Thenumber of history output requests in this ABAQUS analysis (>5000)

maycause SIGNIFICANT performance problems during analysis and postprocessing

輸出項(xiàng)太多,恐硬件資源不夠。要是你確保硬件夠,這條也不怕了。一般的,應(yīng)該減少History中的輸出項(xiàng),盡量輸出你最感興趣的內(nèi)容。

16 Value for parameter nset will be truncatedto 80 characters

nset名字取太長(zhǎng)了,80字符限制

17 compilation - ifort.exe 問(wèn)題

Problemduring compilation - ifort.exe not found in PATH.

安裝的時(shí)候沒(méi)有裝好或是二次開(kāi)發(fā)版本沖突。檢查環(huán)境變量的設(shè)置;然后

verify一下,看看是子程序功能否能通過(guò)?

C系列

如上所說(shuō),有很多warning并一定意味著你的模型存在問(wèn)題。常被問(wèn)起的有:

1 負(fù)特征值問(wèn)題

THE SYSTEM MATRIXHAS 8 NEGATIVE EIGENVALUES.

負(fù)特征值是非線性分析的必然產(chǎn)物。所以不必大驚小怪,甚至久而久之,對(duì)于你熟悉的問(wèn)題,你都會(huì)視而不見(jiàn)了。若出了問(wèn)題,可先檢查下有沒(méi)有伴隨的

numerical sigularity(數(shù)值奇異)和 Zero pivot(零主元)產(chǎn)生。如果沒(méi)有,可以參考這幾個(gè)方面:

1).剛體位移

2).單元異常,過(guò)度變形、過(guò)度扭曲等

3).應(yīng)力應(yīng)變關(guān)系有負(fù)斜率

4) 如果有流體的話,在容器發(fā)生形變的話,也可能出現(xiàn)negative eigenvalue

的情況,不過(guò)不會(huì)出現(xiàn)警告,這是被允許的

5) 失穩(wěn)發(fā)生

2 The ratio ofdeformation speed to wave speed exceeds 1.0000

這個(gè)警告是指單元形變速度V(單元最大形變率/特征尺寸)和膨脹波速C

(通過(guò)材料本構(gòu)關(guān)系求得)的比例超過(guò)1。

解決這個(gè)問(wèn)題的方案有以下幾種:

(1)檢查單位是否封閉(參數(shù)設(shè)置有數(shù)量級(jí)的錯(cuò)誤),此錯(cuò)誤新手常犯;

(2) 檢查網(wǎng)格質(zhì)量 ;

(3) 檢查加載速度,如果條件允許的話就降低速度,該方法也很有效,但在很多

情況下無(wú)法降低速度;

(4) 調(diào)整STEP中的TIME SCALING FACTOR;調(diào)整STEP中的

MASSSCALING FACTOR;

(5) 加*SECTION CONTROLS,NAME=SC,DISTORTION CONTROL,

LENGTHRATION=0.1

或者YES也可以,加在MATERIAL 前面;或加* DIAGNOSTICS,

DEFORMATIONSPEED CHECK=OFF;

或者加*DIAGNOSTICS, CUTOFF RATIO=RATIO(具體數(shù)值),在其他

方法修改后還有問(wèn)題的的情況下使用增加

關(guān)鍵字的方法見(jiàn)http://forum.simwe.com/thread-862510-1-1.html(17樓)

3 zero force/ZERO MOMENT問(wèn)題

THEREIS ZERO MOMENT EVERYWHERE IN THE MODEL BASED ON THE DEFAULT

CRITERION.PLEASE CHECK THE VALUE OF THE AVERAGE MOMENT DURING THE

CURRENTITERATION TO VERIFY THAT THE MOMENT IS SMALL ENOUGH TO BE

TREATEDAS ZERO. IF NOT, PLEASE USE THE SOLUTION CONTROLS TO RESET

THECRITERION FOR ZERO MOMENT.

這個(gè)警告是告訴你模型中沒(méi)有彎矩,沒(méi)問(wèn)題的,可以繼續(xù)計(jì)算。

如果提示中出現(xiàn)特征值奇異的時(shí)候才是計(jì)算有可能出現(xiàn)不收斂的問(wèn)題。

4 Degree of freedom 4 isnot active in this model and can not be restrained

有限元軟件計(jì)算對(duì)于實(shí)體步考慮轉(zhuǎn)動(dòng)自由度,所以你在邊界條件中限制了456的自由度后,軟件會(huì)忽略的啊.

5 The option*boundary,type=displacement has been used; check status file between steps forwarnings on any jumps

prescribedacross the steps in displacement values of translational dof. For rotationaldof make sure that there are

nosuch jumps.All jumps in displacements across steps are ignored.

你采用了位移邊界條件,但在平動(dòng)自由度上,可能在不同的分析步驟里面有突變(你可以從sta文件里面查看),

并且應(yīng)保證轉(zhuǎn)動(dòng)自由度無(wú)突變。通知性質(zhì)的warning,一般是因?yàn)槟悴捎梦灰萍虞d方式,都出這個(gè)。

6 The strain increment hasexceeded fifty times the strain to cause first yield at 377 points

檢查下約束夠不夠,約束夠了就不用管了,這只是通知你,你的模型塑性應(yīng)變很大,一般沒(méi)多大問(wèn)題。

7 123 nodes are usedmore than once as a slave node in *TIE keyword.One of the *TIE constraints ateach of these

nodeshave been identified in node set WarNodeOverconTieSlave

定義接觸的時(shí)候,公共節(jié)點(diǎn)重復(fù)定義了好幾次,這樣可能會(huì)出現(xiàn)過(guò)約束問(wèn)題(只是可能影響)..

8 There are 2unconnected regions in the model.

可能是接觸面由空隙,最好在接觸屬性中定義一個(gè)容差范圍。一般各個(gè)parts之間定義接觸,aba都會(huì)這樣通知用戶的,只要接觸設(shè)置對(duì)了, 一般沒(méi)事。

9 Boundaryconditions are specified on inactive dof of 124 nodes.

Thenodes have been identified in node set WarnNodeBCIactiveDof

邊界條件定義的有問(wèn)題:在124個(gè)節(jié)點(diǎn)的非自由度上有邊界加載

10 The plasticity/creep/connectorfriction algorithm did not converg

一般是塑性應(yīng)變太大,單元扭曲導(dǎo)致的。可以先改為彈性模型看看是否收斂;

11 The ratio of the maximum incrementaladjustment to the average characteristic

lengthis 1.82846e-02 at node 10868 instance jiti1 on the surface pair(assembly_jq22,assembly_q22).

可以通過(guò)調(diào)大預(yù)設(shè)值消除該提示and檢查網(wǎng)格質(zhì)量。

12 ELEMENT 42 INSTANCE SOIL3-1 ISDISTORTING SO MUCH THAT IT TURNS

應(yīng)改進(jìn)單元質(zhì)量

13 650nodes are either missing intersection with their respective master surface oroutside the adjust zone.

改改tie里的tolarance試試

14 Dependentpart instances cannot be edited or assigned mesh attributes

模型樹(shù)--assembly-打擊part 右鍵--make independent。也可以到模型樹(shù)part步展開(kāi)點(diǎn)mesh。

15 Theaspet ratio for nnn elements exceeds 100 to 1.

單元?jiǎng)澐志W(wǎng)格長(zhǎng)寬比不合適。如果這些單元在不重要的區(qū)域(對(duì)結(jié)果肯定有些影響,

影響大小取決于這三個(gè)單元的位置,在模型中的作用等),而且能計(jì)算,那就沒(méi)問(wèn)題了

16 123 elementsare distorted

存在單元扭曲,如果這些單元在不重要的區(qū)域(對(duì)結(jié)果肯定有些影響,

影響大小取決于這三個(gè)單元的位置,在模型中的作用等),而且能計(jì)算,那就沒(méi)問(wèn)題了(同15)

17 ***WARNING: DEGREE OF FREEDOM 1 IS NOTACTIVE ON NODE 6 - THIS BOUNDARY

CONDITIONIS IGNORED

約束了單元沒(méi)有得自由度對(duì)求解沒(méi)有影響,可以查看下

18 熱分析時(shí)出現(xiàn)了這樣的警告“THERE IS ZERO HEAT FLUX EVERYWHERE

Thereis 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 issmall enough to be treated as zero.

ifnot, please use the solution controls to reset the criterion for zero HEATFLUX.

試試:

(1)是不是熱源定義的問(wèn)題,錯(cuò)誤信息是說(shuō)熱源量幾乎為零。

(2)定義熱源的子程序調(diào)用命令流應(yīng)該為*HEAT GENERATION,在材料模塊中定義,子程序?yàn)?/span>HETVAL。

19 The elements in the element setWarnElemSurfaceIntersect-Step1 are involved

surfaceintersections. Refer to the status and message file for further details

檢查一下你單元集合的定義以及面的定義,看是否出現(xiàn)了相交或重復(fù)定義的情況

20 Boundary conditions arespecified on inactive dof of 36 nodes. The nodes have been identified in nodeset

WarnNodeBCInactiveDof.

21 Integration and section pointoutput variables will not be output for deformable elements that are declaredas rigid using the

*rigidbody option

這個(gè)僅是通知性質(zhì)的(在interaction步設(shè)置為rigid body,不輸出應(yīng)力應(yīng)變),你在interaction步定義了剛體約束的話,都會(huì)出這個(gè)警告。

22 For a self contactsurface, the facets of the elements in element setWarnElemFacetThickPt63d-Step1 are thicker than 0.6 times

anedge or diagonal length

ofthe facets. Use the MAXRATIO parameter on *SURFACE DEFINITION to allowautomatic rescaling of the contact

thicknesseswhere necessary for this surface.

Referto the status file for furtherdetails.

23 NO VALID RADIATION OUTPUTREQUESTS HAVE BEEN GENERATED. THIS MAY BE DUE TO EARLIER INPUT ERRORS ORSPECIFICATION

OFA NONEXISTANT CAVITY OR SURFACE NAME

檢查一下你的output設(shè)定裡是不是有些set或surface沒(méi)有設(shè)定到

24 123 nodes may haveincorrect normal definitions. The nodes have been identified in node setWarnNodeIncorrectNormal。

先用看看WarnNodeIncorrectNormal在哪兒。這個(gè)不一定是致命的警告,有時(shí)候可以忽略。如果模型不收斂,可以檢查下是否有過(guò)約束,

在接觸上存在邊界條件or加載。

D系列

----------------------------------------------------------------------------------------------------------

ERROR:Toomany attamps have been made

Toomany attamps have been made....

THESOLUTION APPEARS TO BE DIVERGING.

CONVERGENCEISJUDGED UNLIKELY.

TIMEINCREMENT REQUIRED IS LESS THAN THE MINIMUM SPECIFIED

AnalysisInput File Processor exited with an error.

-----------------------------------------------------------------------------------------------------------

這樣的信息幾乎是無(wú)用信息(除了告訴你的模型分析失敗以外,沒(méi)有告訴你任何有用的東西)。宜再查找別的信息來(lái)考察。比如:

1 ) Numerical sigularity solver problem. numerical sigularity

whenprocessing node105 instance 表示:數(shù)值奇異:剛體位移(欠約束)

2) Zero pivot 表示:過(guò)約束

這樣的信息(當(dāng)然不僅僅是這些),才是比較有價(jià)值的。

2 對(duì)于TIME INCREMENT REQUIRED IS LESSTHAN THE MINIMUM SPECIFIED

Toomany attamps have been made

3 對(duì)于“網(wǎng)格扭曲”的警告: excessively distortedelements 前面有提到。

第一步:采用二樓底下的方法用display查看“ ErrElemExcessDistortion-Step1 ”在模型的哪些部位,做到心中有數(shù)。

第二步:檢查模型的網(wǎng)格質(zhì)量:mesh步---verify----AnalysisCheck選取模型。這種情況,一開(kāi)始計(jì)算即出現(xiàn)“distorted element”的信息。Besides:很多其他問(wèn)題也會(huì)網(wǎng)格扭曲警告。比如,幾何模型導(dǎo)入有誤需要修補(bǔ)、單元類型選取錯(cuò)誤、邊界條件有誤、材料屬性錯(cuò)誤、接觸設(shè)置不合理、子程序錯(cuò)誤等。

第三步:即使你的網(wǎng)格劃分很好,如果變形過(guò)大,也會(huì)導(dǎo)致網(wǎng)格扭曲。然后修改網(wǎng)格劃分,怒要出現(xiàn)紅色,關(guān)鍵區(qū)域不要出現(xiàn)黃色。(當(dāng)然最好是所有的網(wǎng)格都用structure劃分,且都沒(méi)有紅色、黃色出現(xiàn)。網(wǎng)格質(zhì)量就比較好。這種情況,警告信息往往是在計(jì)算到一定步驟之后才出現(xiàn)“distorted element”。這種情況建議采用ALE等方式,此不詳述,搜索論壇“網(wǎng)格重劃”“ALE”等技術(shù)。

開(kāi)放分享：優(yōu)質(zhì)有限元技術(shù)文章,助你自學(xué)成才