关于接触初始间隙的处理求助各位
我用下面的命令流生成简单的解除对，然后进行自重下的静力计算，但在已开始的接触面检查上就提示接触面是open的，这样的话计算肯定是不能收敛的，但我按照help中的调整了实常数，还是没法消除这个gap，请问该如何处理啊？命令流：
/CONFIG,NRES,2000000
/PREP7
ET,1,PLANE182, , ,2 ! 2-D PLANE-STRAIN 4-NODE STRUCTURAL SOLID
KEYOPT,1,6,1 ! Mixed U-P FORMULATION
ET,2,TARGE169 ! 2-D TARGET ELEMENT
ET,3,CONTA171 ! 2-D CONTACT ELEMENT
KEYOPT,3,5,4
KEYOPT,3,10,1
!KEYOPT,3,12,1
R,1,0,0,0.01, 0,0,0
RMORE,,,1e20, ,,1
RMORE,0,,, ,,
RMORE,,,, ,,
MP,EX,1,2.82e13 ! YOUNG'S MODULUS
MP,NUXY,1,0.2 ! POISSON'S RATIO
MP,DENS,1,2000
MP,MU,1,0.5 !FRICTION COEFFICIENCE
!rectng,0,2,0,1
rectng,-1,1,0,1
k,100,-2
k,101,2
l,100,101
asel,s,area,,1
TYPE,1
mat,1
esize,0.1
AMESH,ALL ! MESH AREA 1
REAL,2
TYPE,2
LMESH,5
REAL,2
TYPE,3
LMESH,1
FINI
/SOLU
antype,static
SOLCONTROL,on
NSUBST,100
KBC,0
ACEL,0,10,0,
autos,on
lsel,s,line,,5
nsll,s,1
d,all,all
allsel,all
solve
fini
检查文件：
*** NOTE *** CP = 42.479 TIME= 23:25:37
Rigid-deformable contact pair identified by real constant set 2 and
contact element type 3 has been set up.Please verify constraints on
target nodes which may be automatically fixed by ANSYS.
Contact algorithm: Augmented Lagrange method
Contact detection at: Gauss integration point
Default contact stiffness factor FKN 1.0000
The resulting contact stiffness 0.56400E+16
Default penetration tolerance factor FTOLN 0.10000
The resulting penetration tolerance 0.10000E-01
Max. initial friction coefficient MU 0.50000
Default tangent stiffness factor FKT 1.0000
Default elastic slip factor SLTOL 0.10000E-01
The resulting elastic slip 0.10000E-02
Update contact stiffness for each sub-load step
Default Max. friction stress TAUMAX 0.10000E+21
Average contact surface length 0.10000
Average contact pair depth 0.10000
Default pinball region factor PINB 1.5000
The resulting pinball region 0.15000
Automatic initial closure factor ICONT 0.0000
The resulting initial contact closure 0.0000
*WARNING*: Automatic adjustment can cause severe discontinuity
*WARNING*: Initial penetration is included.
*** NOTE *** CP = 42.479 TIME= 23:25:37
No contact was detected for this contact pair.
****************************************
*** WARNING *** CP = 42.479 TIME= 23:25:37
All selected contact pairs are initially open.Rigid body motion can
occur.You may use auto CNOF/ICONT by setting KEYOPT(5) to close
small gaps.
*** WARNING *** CP = 42.510 TIME= 23:25:38
Max.Friction coef.0.5 is defined in the model.Switch to the
unsymmetric solver (NROP,UNSYM) instead if convergence difficulty is
encountered.
1 CONTACT PAIR IS SELECTED
CONTACT PAIR HAVING REAL ID = 2 IS INITIALLY OPEN
BUT MAY BE AUTOMATICALLY CLOSED
我按照help中的方法调整了相关实常数以及OPTION（5）和OPTION（12）都没消除掉！！！所以想请教下各位这个基本的问题，这个不解决，我没法继续下去了！再次谢谢！
自己回答下，发现错误在于生成线的命令：
k,100,-2
k,101,2
l,100,101
应该是：l,101,100，这样能确保目标面的外法线方向是向上，指向接触单元的。上面的命令使目标面的外法线方向向下，背离了接触面单元，因此，程序检测出接触有间隙！
页:
[1]