abaqus出現(xiàn)Too many attempts made for this increment怎么解決？

2017-06-14 by:CAE仿真在線來源:互聯(lián)網(wǎng)

abaqus會進程碰到Too many attempts made for this increment,如下圖

ABAQUS中出現(xiàn)Too many attempts made for this increment錯誤是什么原因?abaqus有限元圖片1

Threre may be many factors that you should check. Some of them you might want to check predominantly are,1_Material properties and equivalency of units 2_ Mesh size and type 3_Boundary conditions 4_constraints such as rigid body motion 5_Step size and no of increments Also look in Abaqus documentation for Common problems in convergence of solution.

模擬計算的加載過程包含單個或多個步驟,所以要定義分析步。它一般包含分析過程選擇,載荷選擇,和輸出要求選擇。而且每個分析步都可以采用不同的載荷、邊界條件、分析過程和輸出要求。例如:步驟一:將板材夾于剛性夾具上。步驟二:加載使板材變形。步驟三:確定變形板材的自然頻率。增量步是分析步的一部分。在非線性分析中,一個分析步中施加的總載荷被分解為許多小的增量,這樣就可以按照非線性求解步驟來進行計算。當提出初始增量的大小后,ABAQUS會自動選擇后繼的增量大小。每個增量步結(jié)束時,結(jié)構(gòu)處于(近似)平衡狀態(tài),結(jié)果可以寫入輸出數(shù)據(jù)庫文件、重啟動文件、數(shù)據(jù)文件或結(jié)果文件中。選擇某一增量步的計算結(jié)果寫入輸出數(shù)據(jù)庫文件的數(shù)據(jù)稱為幀。迭代步是在一增量步中找到平衡解的一種嘗試。如果模型在迭代結(jié)束時不是處于平衡狀態(tài),ABAQUS將進行另一輪迭代。隨著每一次迭代,ABAQUS得到的解將更接近平衡狀態(tài);有時ABAQUS需要進行許多次迭代才能得到一平衡解。當平衡解得到以后一個增量步才完成,即結(jié)果只能在一個增量步的末尾才能獲得。

step,increment,attempt,iteration,的關系
1)step 分析步
2)increment 時間增量步
3)attempt 減小增量步的嘗試,即“cutback”
4)iteration 迭代
在一個計算中有可能用到多步分析,比如建一個土石壩,每激活(add)一個填筑層就是一個分析步step;
在每個step中,如果考慮非線性,step就會分成幾個增量步(increment)進行計算;
在每個increment中,會有減小增量步的嘗試(attempt),在每個attemp中,要進行迭代計算(iteration)。
如果迭代收斂,則在下一個increment中會增大時間增量步(比如第一個increment=0.2,則下一個會增大為0.3)
如果迭代無法達到收斂,則ABAQUS會自動減小時間增量步(減小increment),即所謂的“cutback”,如果仍然不能收斂,則會繼續(xù)減小時間增量步,默認的cutback最大次數(shù)為5次,也就是attempt最大=5,如果5次之后仍不能收斂則ABAQUS會停止分析,顯示錯誤:too many attempts made for this increment:analysis terminated.
increment時間增量步有最小值,默認的是1e-5,如果increment減小到比這還小,ABAQUS就會停止分析,出現(xiàn)錯誤:time increment required is less than the minimum specified.
increment的值可以在關鍵字*static中修改:
*static 1., 1., 1e-05, 1.
分別為初始增量步,分析時間步,最小增量步,最大增量步
可以用關鍵字*Step設定一個分析步中increment的最大步數(shù),如:
*Step,INC=600 (the maximum number of increments in a step,默認的是100 )
*static和*Step中的increment是相同的,*Step,INC默認為100,而*static中默認為1e-5,并不是100*(1e-5)=1,這兩個數(shù)都是限值,即number of increments最大為100,而increment最小為1e-5。

這種問題怎么解決呢?

算了三個非線性混凝土節(jié)點模型,兩個通過,其中一個出現(xiàn)“TOO MANY ATTEMPTS MADE FOR THIS INCREMENT”錯誤。查了一下論壇中的解決方案,知道是ABAQUS默認的Cutback最大次數(shù)為5次的限制出現(xiàn)上述錯誤信息。
問題:怎樣修改這個ABAQUS默認的Cutback最大次數(shù)為5次的限制,因為我的minmun increment size是1e-07,最后計算狀態(tài)是:
2 2775 1U 0 9 9 8.67 7.67 0.08653
2 2775 2U 0 5 5 8.67 7.67 0.02163
2 2775 3U 0 6 6 8.67 7.67 0.005408
2 2775 4U 0 6 6 8.67 7.67 0.001352
2 2775 5U 0 4 4 8.67 7.67 0.0003380

THE ANALYSIS HAS NOT BEEN COMPLETED
還遠沒有達到我的minmun increment size=1e-07的限制,如果修改默認的Cutback最大次數(shù),可能可以收斂。

.........
** CONTROLS
**
*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 10, , ,
**
** OUTPUT REQUESTS
..........
上面inp文件中參數(shù)10就是我把原來缺省的Cutback最大5次限制設置到了10次
希望對各位有幫助,我試過了,可以收斂了。

** BOUNDARYCONDITIONS
**
.........
** CONTROLS
**
*Controls, reset
*Controls, parameters=time incrementation
, , , , , , , 10, , ,
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
**FIELDOUTPUT: F-Output-1
**
*Output, field, frequency=3
*Node Output

那要怎么修改這個值呢?

可以參考下圖,先導出inp,修改inp,在通過inp創(chuàng)建job,然后再執(zhí)行即可

abaqus出現(xiàn)Too many attempts made for this increment怎么解決？abaqus有限元培訓教程圖片2

abaqus出現(xiàn)Too many attempts made for this increment怎么解決？abaqus有限元培訓教程圖片3

這樣可以定位了在** BOUNDARY CONDITIONS和*Restart, write, frequency=0
之間

一般aba的分析精度到E-5,若是小于這個數(shù)量級還是不收斂,那么你幾時改小了初始時間增量,能計算出來,結(jié)果的可靠性還是大打折扣。

個人認為,出現(xiàn)這種問題,屬于嚴重的不收斂問題,最好還是從模型上找出原因,肯定是模型上有一些影響收斂的錯誤。

還有另一種原因,可能是發(fā)生了計算過程中結(jié)果材料損傷嚴重塑性變形進行高度非線性,這樣的話那么abaqus/Standard里面的隱式分析,速度很很受影響,也會出現(xiàn)收斂困難或者不收斂的問題,對于動力分析來講,可以考慮采用abaqus/Explicit的顯式積分算法,倒是一個不錯的選擇。

=========================

hey all,

I am using the macro tool to record myself importing geometry and then setting up contact between parts automatically.

Then I change the 2d iges files I am importing using another cadpackage(catia) and am trying to get a contatc analysis to run with the specific geometry I have imported.

Anyway the problem I am having is that sometimes when I import the new gemetry and submit ajobit works and other times I get the error 'too many attempts made for this increment error'

I am quite confused and hoping someone may know what this means;

using a stabilize option can be a correct solution but take care using this option because it can also help convergence of an analysis by giving unphysical results.

The way of solving problems is to check all infos in your .msgfile:
first by running an analysis with *PREPRINT,CONTACT=YES in the model part of your .inp (between *HEADING and the first STEP) and adding *CONTACT PRINT in each step.

your analysis will give you very big .dat and .msg files with full info about all the contacts in the model.

Then many options :
- you read the contact details and detect "chattering" : a second order node opens, closes, opens, etc ... through the increments. Then use a more appropriate element type (linear element or 2nd order modified element - for example C3D10M instead of a C3D10)
- if you see that nearly all your contacts are realized and few are still opened or closed, you can allow code to make more attempts in step by using the *CONTROLS card (be careful this area is full of parameters, check it twice before re-running analysis) the default must be about 5 attempts you can define a bit more
- if you noticed a large occurence of the word "overclosure" followed by tiny values (i-e 1E-7) AND if your loading/boundary condition is not too large, you can switch the automatic tolerances by *CONTACT CONTROLS, AUTOMATIC TOLERANCES in the step part. ((reset to *CONTACT CONTROLS, RESET) in the next step .

To limit the problems with contact always try to use displacement approach instead of FOrce approach if possible.

HI
I am a MSc student from BUET . i am modelling a Rcc beam using ABAQUS.The dimension of the beam is 200mmX300mmX3000mm. i choosed elemnt size 200mmX30mmX50mm . Used the general static step.

for concrete i euse
*elastic
33000, 0.2
*concrete
17.4,0? (i used 17.4=0.45*.85*f'c=fy)
34.5,0.0029 ? (34.5= 0.85*fic)
*tension stiffening
1,0
0,0.193
*FAILURE RATIOS
1.16 ,0.09,1.28,0.333

for steel i am using
*elastic
200000,0.31
*PLASTIC
439.964,0
753.13,0.1785
*embedded element,host elset=all_conc_elements
reinforcement

the problem is , i am getting much stiffer result. the initial portion of the load displacement curve is at a much higher (load almost double) position. i am also not getting the displacement correct. i get result up to 10 mm of displacement but the experimental curve has 80 mm displacement. In the msg file i find the same message everytime Too many attempts made for this increment. also there are negetive eigen values.

If any one can suggest me about this stiffer result, it would be a great help

開放分享：優(yōu)質(zhì)有限元技術文章,助你自學成才