不能收敛（目前已解决，并附流文件）

alex_shoal

在进行简支梁分析的时候碰到一个问题，反复尝试不知道是什么原因导致不能收敛。
弹出信息
“one or mor elements have become highly distorted.excessive distortion of element is usually a symptom indicating the need for corrective action elsewhere....."
希望路过的高手指点迷津，拜谢
具体命令流
FINISH
/CLEAR,NOSTART
/COM, Structural  

!*********** parameter setup **************
B_WIDTH=0.46  !WIDTH & THICKNESS & LENGTH OF THE BEAM
B_LEN=13.7
B_THK=0.3
S_WIDTH=0.6   !WIDTH & THICKNESS & LENGTH OF THE SUPPORT
S_LEN=0.6
S_THK=0.3
DISTANCE=-1-B_THK/2-S_THK/2 !distance between beam and support surface.
MESH_OFFSET=0.8
DISP_OFFSET=4.5
YIELD=700
TANG_MODE=800
COF=0
!control the element size
THK_DIVISOIN=4
WIDTH_DIVISION=3
V_CONTACTG_SIZE=0.1
V_TRANS_SIZE=0.2
V_BEAN_SIZE=0.2

!*********** parameter setup end **************
/PREP7
!*****Material Setup
ET,1,SOLID45
EX,1,1.126E5
NUXY,1,0.35
TB,BISO,1,1,2,  
TBDATA,1,YIELD,TANG_MODE,,,
!*****Create Model

BLC5,0,0,B_WIDTH,B_THK,B_LEN  !CREATE BEAM
BLC5,0,0,S_WIDTH,S_THK,S_LEN  !CREATE SUPPORT
/PNUM,KP,0  
/PNUM,LINE,1
/PNUM,AREA,1
/PNUM,VOLU,0
/PNUM,NODE,0
/PNUM,TABN,0
/PNUM,SVAL,0
/NUMBER,0   
!*  
/PNUM,ELEM,0

VGEN, ,2, , , ,DISTANCE, , , ,1  !MOVE SUPPORT TO NEW LOCATION
WPAVE,0,0,DISP_OFFSET
VSBW,ALL                         !get the displacement apply position
WPAVE,0,0,0
WPAVE,0,0,MESH_OFFSET
VSBW,ALL                         !get contact surface offset area.

!element size Setup
LESIZE,1, , ,THK_DIVISOIN
LESIZE,2, , ,WIDTH_DIVISION
LESIZE,9, V_CONTACTG_SIZE
LESIZE,41,V_TRANS_SIZE
LESIZE,36,V_BEAN_SIZE
!*****mesh
VSEL,S,LOC,Y,-0.5,1
VSWEEP,ALL

!create the contact pair.
MP,MU,1,COF !set cof
MAT,1   
R,3
REAL,3  
ET,2,170
ET,3,174
KEYOPT,3,9,0
KEYOPT,3,10,2   
!R,3,
!RMORE,  
!RMORE,,0
!RMORE,0
! Generate the target surface   
ASEL,S,,,8  
ASEL,A,,,10
!CM,_TARGET,AREA
AATT,-1,3,2,-1  
TYPE,2  
AMESH,ALL
!Generate the contact surface  
ASEL,S,,,6
ASEL,A,,,1
TYPE,3  
NSLA,S,1
ESLN,S,0
ESURF   
!*****apply the load
/SOL
DL,29, ,UY,-2
NSEL,S,LOC,Z,B_LEN
D,ALL,ALL,
ANTYPE,0
NLGEOM,1
NSUBST,100,1000,25
OUTRES,ERASE
OUTRES,ALL,ALL  
TIME,1
ALLSEL,ALL  
/VIEW,1,1,2,3   
/ANG,1
/REPLOT
/VIEW,  1, -0.777520041429    ,  0.375984275955    , -0.504081748739
/ANG,   1,   3
save
!*****solve
solve

!*****POST
/POST1
SET,,, ,,, ,1
PLNS,S,EQV  
ANTIME,10,0.5, ,1,0,0,1

[ 本帖最后由 alex_shoal 于 2007-4-19 09:52 编辑 ]

newton

我感觉模型的问题.



接触的两刚性面需要圆角过渡,同时发生接触部位应网格局部加密

[ 本帖最后由 newton 于 2007-4-14 00:09 编辑 ]

alex_shoal

我加了个圆角
居然收敛了。
哈哈
谢谢，
附

FINISH
/CLEAR,NOSTART
/COM, Structural  

!*********** parameter setup **************
B_WIDTH=0.46  !WIDTH & THICKNESS & LENGTH OF THE BEAM
B_LEN=13.7
B_THK=0.3
S_WIDTH=0.6   !WIDTH & THICKNESS & LENGTH OF THE SUPPORT
S_LEN=0.4
S_THK=0.3
Round=0.05

DISTANCE=-1-B_THK/2-S_THK/2 !distance between beam and support surface.
MESH_OFFSET=0.8
DISP_OFFSET=4.5
YIELD=700
TANG_MODE=800
COF=0
!control the element size
THK_DIVISOIN=4
WIDTH_DIVISION=3
V_CONTACTG_SIZE=0.1
V_TRANS_SIZE=0.2
V_BEAN_SIZE=0.2

!*********** parameter setup end **************
/PREP7
!*****Material Setup
ET,1,SOLID45
EX,1,1.126E5
NUXY,1,0.35
!TB,BISO,1,1,2,  
!TBDATA,1,YIELD,TANG_MODE,,,
!*****Create Model
!CREATE BEAM
BLC5,0,0,B_WIDTH,B_THK,B_LEN  
!CREATE SUPPORT
BLC5,0,0,S_WIDTH,S_THK,S_LEN
WPAVE,0,0,S_LEN
BLC5,0,Round*(-0.5),S_WIDTH,S_THK-Round,Round
WPAVE,S_WIDTH/2,(S_THK/2-Round),S_LEN
WPRO,,,-90
CYL4,0,0,Round,,,,S_WIDTH
VADD,2,3
VADD,4,5
/PNUM,KP,0  
/PNUM,LINE,1
/PNUM,AREA,1
/PNUM,VOLU,0
/PNUM,NODE,0
/PNUM,TABN,0
/PNUM,SVAL,0
/NUMBER,0   
!*  
/PNUM,ELEM,0

VGEN, ,2, , , ,DISTANCE, , , ,1  !MOVE SUPPORT TO NEW LOCATION

WPAVE,0,0,0
WPCSYS,-1,0,
WPAVE,0,0,DISP_OFFSET
VSBW,ALL                         !get the displacement apply position
WPAVE,0,0,0
WPCSYS,-1,0
WPAVE,0,0,MESH_OFFSET
VSBW,ALL                         !get contact surface offset area.

!element size Setup
LESIZE,1, , ,THK_DIVISOIN
LESIZE,2, , ,WIDTH_DIVISION
LESIZE,9, V_CONTACTG_SIZE
LESIZE,61,V_TRANS_SIZE
LESIZE,50,V_BEAN_SIZE
!*****mesh
VSEL,S,LOC,Y,-0.5,1
VSWEEP,ALL

!create the contact pair.
MP,MU,1,COF !set cof
MAT,1   
R,3
REAL,3  
ET,2,170
ET,3,174
KEYOPT,3,9,0
KEYOPT,3,10,2   
R,3,0.02,0,0.1,0.1,0.0
! Generate the target surface   
ASEL,S,,,15  
ASEL,A,,,30
ASEL,A,,,17
!CM,_TARGET,AREA
AATT,-1,3,2,-1  
TYPE,2  
AMESH,ALL
!Generate the contact surface  
ASEL,S,,,6
ASEL,A,,,1
TYPE,3  
NSLA,S,1
ESLN,S,0
ESURF   
!*****apply the load
/SOL
DL,30, ,UY,-2
NSEL,S,LOC,Z,B_LEN
D,ALL,ALL,
ANTYPE,0
NLGEOM,1
NSUBST,100,1000,25
OUTRES,ERASE
OUTRES,ALL,ALL  
TIME,1
ALLSEL,ALL  
/VIEW,1,1,2,3   
/ANG,1
/REPLOT
/VIEW,  1, -0.777520041429    ,  0.375984275955    , -0.504081748739
/ANG,   1,   3
save
!*****solve
solve

!*****POST
/POST1
SET,,, ,,, ,1
PLNS,S,EQV  
ANTIME,10,0.5, ,1,0,0,1

[ 本帖最后由 alex_shoal 于 2007-4-19 09:50 编辑 ]

alex_shoal

另外一种收敛的方法。

!*********** parameter setup **************

B_WIDTH=0.46  !WIDTH & THICKNESS & LENGTH OF THE BEAM
B_LEN=13.7
B_THK=0.3

S_WIDTH=0.6   !WIDTH & THICKNESS & LENGTH OF THE SUPPORT
S_LEN=0.6
S_THK=0.3

DISTANCE=-1-B_THK/2-S_THK/2 !distance between beam and support surface.

MESH_OFFSET=0.8
DISP_OFFSET=4.5

YIELD=700
TANG_MODE=800
COF=0

!control the element size
THK_DIVISOIN=4
WIDTH_DIVISION=3

V_CONTACTG_SIZE=0.1
V_TRANS_SIZE=0.2
V_BEAN_SIZE=0.2


!*********** parameter setup end **************
/PREP7

!*****Material Setup
ET,1,SOLID45
EX,1,1.126E5
NUXY,1,0.35
TB,BISO,1,1,2,  
TBDATA,1,YIELD,TANG_MODE,,,

!*****Create Model

BLC5,0,0,B_WIDTH,B_THK,B_LEN  !CREATE BEAM
BLC5,0,0,S_WIDTH,S_THK,S_LEN  !CREATE SUPPORT

/PNUM,KP,0  
/PNUM,LINE,1
/PNUM,AREA,1
/PNUM,VOLU,0
/PNUM,NODE,0
/PNUM,TABN,0
/PNUM,SVAL,0
/NUMBER,0   
!*  
/PNUM,ELEM,0


VGEN, ,2, , , ,DISTANCE, , , ,1  !MOVE SUPPORT TO NEW LOCATION
WPAVE,0,0,DISP_OFFSET
VSBW,ALL                         !get the displacement apply position
WPAVE,0,0,0
WPAVE,0,0,MESH_OFFSET
VSBW,ALL                         !get contact surface offset area.


!element size Setup

LESIZE,1, , ,THK_DIVISOIN
LESIZE,2, , ,WIDTH_DIVISION
LESIZE,9, V_CONTACTG_SIZE
LESIZE,41,V_TRANS_SIZE
LESIZE,36,V_BEAN_SIZE

!*****mesh
VSEL,S,LOC,Y,-0.5,1
VSWEEP,ALL



!create the contact pair.
MP,MU,1,COF !set cof
MAT,1   
R,3
REAL,3  
ET,2,170
ET,3,174

KEYOPT,3,9,0
KEYOPT,3,10,2   

! make the beam the target surface

allsel
type,1
real,1
mat,1
esel,none
nsel,none
vmesh,2
d,all,all

Real,3
TYPE,3  
ESURF  

allsel

type,2
amesh,6

!*****apply the load

/SOL
DL,29, ,UY,-2
NSEL,S,LOC,Z,B_LEN
D,ALL,ALL,

ANTYPE,0
NLGEOM,1
NSUBST,100,1000,25
OUTRES,ERASE
OUTRES,ALL,ALL  
TIME,1
ALLSEL,ALL  
/VIEW,1,1,2,3   
/ANG,1
/REPLOT
/VIEW,  1, -0.777520041429    ,  0.375984275955    , -0.504081748739
/ANG,   1,   3
save

!*****solve

solve


!*****POST

/POST1

SET,,, ,,, ,1
PLNS,S,EQV  
ANTIME,10,0.5, ,1,0,0,1

ansyslove

怎么解决的? 介绍以下咯!!

liuq8221

在nolinear convergence criteria对话框中有 VALUE   Rrference value of lab和 TOLER  Tolerance about VALUE两项，这两项是作什么用的啊？
ANSYA默认的收敛精度是0.5%，我想把收敛条件放宽一些比如放宽到5%应该怎么作呀？
楼主知道怎么作吗？

ansyslove

我想他不知道的 :( :( :( :(