Ansys里面如何将一个立方体设为刚体?

一、ANSYS WORKBENCH环境下

在ANSYS WORKBENCH可以将一个立方体设为刚体，根据如下：

二、ANSYS MECHANICAL APDL(经典界面）环境下

   在该环境下，似乎不能将一个立方体设为刚体，一般通过其他途径实现刚体的位移效果。现分别列举3D和2D刚体模型说明使用方法。

 1、3D刚性圆柱体冲切金属块

      下例使用了2种建立接触单元的方法：直接法AMESH(适用于之前AREA上没有单元及节点情况）；覆盖法（ESURF)（适用于之前AREA上已经生成了其他实体单元的节点）；

Metal Forging Simulation：

/batch,list
/config,nproc,1
/PREP7
!-----------geometry parameters---------------  !mm
cylinder_radius         =       500     
cylinder_offset         =       1000    
block_height            =       1000    
radius_fillet           =       33
!---------inital meshing parameters------------
block_esize                     =       200                     
cylinder_esize          =       200                     
!------------loading parameters----------------
cylinder_disp           =       -800            
!------------NLAD parameters------------------
skw_                    =       0.9                                             !skewness threshold
freq                    =       1                                                       !NLAD frequency (1 means check every substep)
start_time              =       0                                               !beginning time for NLAD interval
end_time                =       1                                                       !end time for NLAD interval
!------------remeshing parameters---------------
sculpt_layers   =       2                                               !number of sculpting layers
conc_                   =       10                                                      !concave patch splitting angle                                                                                                                  
conv_                   =       10                                                      !convex patch splitting angle
edge_                   =       10                                                      !edge splitting angle

!******************material properties*****************
MP,EX,1,70e3                                                            !aluminium material properties                                                                                                                  
MP,NUXY,1,0.33                                                  !poisson's ratio
MP,MU,1,0                                                                       !coefficient of friction                                                                                                                        
TB,BISO,1,1                                                                     !bilinear isotropic material
TBDATA,1,20                                                                     !yield stress in MPa
TBDATA,2,7e3                                                            !tangent modulus in MPa

!------------geometry creation-------------------
blc4,0,0,block_height,block_height,block_height
k,9,0,cylinder_offset,0
k,10,0,cylinder_offset,cylinder_radius
k,11,0,cylinder_offset+cylinder_offset,cylinder_radius
k,12,0,cylinder_offset+cylinder_offset,0
l,9,10 
l,10,11
l,11,12
l,12,9                       
lfil,13,14,radius_fillet
al,13,17,14,15,16
vrotat,7,,,,,,9,12,90

!---------element types & settings-----------
et,1,285 
et,2,170
et,3,173
!-------------general meshing----------------
type,1
mat,1          
real,1           
esize,block_esize
vmesh,1
!-------------contact pair 1----------------
real,2                     
!---------------target elements--------------
type,2
mat,2                           
asel,s,area,,8,10
aesize,all,cylinder_esize
amesh,all
alls
!---------------contact elements-----------
type,3
mat,1                  
asel,s,area,,4
nsla,s,1
esln
esurf
alls
!--------------create components-----------
esel,s,ename,,285
cm,comp1,elem                           !make whole block as NLAD component
alls
!-----boundary conditions & loading-------      
asel,s,area,,5,6
nsla,s,1
d,all,ux,0.0
alls
asel,s,area,,1,2
nsla,s,1
d,all,uz,0.0
alls
asel,s,area,,3  
nsla,s,1
d,all,uy,0.0
alls
asel,s,area,,7,12
nsla,s,1
d,all,uz,0.0
d,all,ux,0.0
d,all,uy,cylinder_disp
alls
finish

/SOLU                                                                                                                           
!--------------general solution settings--------
nlgeom,on
eresx,no
outres,all,all
!---------------NLAD settings-------------------
!check NLAD parameters section above for values
nlad,comp1,add,mesh,skew,skw_                           !nlad with mesh distortion criterion
nlad,comp1,on,,,freq,start_time,end_time        
!------------remeshing settings---------------
!check remeshing parameters section above for values
nlad,comp1,nlay,sculpt_layers
nlad,comp1,nang,conc_,conv_ 
nlad,comp1,aedg,edge_

!---------------step settings-------------------
time,1  
nsubst,100,10000,10

alls
solve
finish

!---------------POSTPROCESSING-------------------------
/POST1
set,list
finish
/exit

 

 2、2D刚性钢管挤压橡胶塑料

     下例使用了2种建立接触单元的方法：直接法LMESH(适用于之前LINE上没有单元及节点情况）；覆盖法（ESURF)（适用于之前LINE上已经生成了其他实体单元的节点）；

Example: Rubber Seal Simulation：

/batch,list

/prep7

/com geometry paratmeters
rf = 1
yd = 6
yf = 12
xc = 0
yc = 12
disp = -4.0
w = 3

/com element types and size
el = w
et,1,182
keyopt,1,3,2
!keyopt,1,6,1

et,2,169
et,3,171
keyopt,3,9,0
keyopt,3,10,1
!keyopt,3,2,3

/com materials
c10=62.3584129
c01=-37.8485452
dd=1.E-03

tb,hyper,1,,2,mooney
tbdata,1,c10,c01,dd

mp,mu,2,0.0

r,2

/com create the model
k,1,xc,yc
k,2,xc+3*w,yc
k,3,w,0.0
k,4,w,yd
k,5,3*w,yd
rect,0,w,0,yd
rect,0,w,yd,yf
/pnum,line,1
l,1,2
l,3,4
l,4,5
lfillt,10,11,rf

/com create mesh
esize,el
mat,1
type,1
real,1
amesh,1,2
/pnum,elem,1
/pnum,node,1
nummrg,node
numcmp,node
/replot

/com the 1st contact paires
mat,2
real,2
type,2

esize,yf
lmesh,9
allsel,all

type,3  
lsel,,,,6,7 
nsll,,1 
esln,,0 
esurf   
alls

/com the 2nd contact paires
real,3
type,2

lplot
esize,yf
lmesh,9,12
lsel,s,line, ,10,12
esll,s,1
esurf, ,reverse
allsel,all

lplot
type,3  
lsel,,,,6
lsel,a,,,2
nsll,,1 
esln,,0 
esurf   
alls

/com boundary condition

/com rigid punch
lsel,,,,9
nsll,,1
d,all,uy,disp
d,all,ux,0.0
alls

/com rigid die face
lsel,,,,10,12
nsll,,1
d,all,uy,0.0
d,all,ux,0.0
alls

/com left side
nsel,,loc,x,0
d,all,ux,0.0
alls

/com bottom
nsel,,loc,y,0
d,all,uy,0.0
alls

/com check the contact definition
cncheck
elist
fini

/solution

/com define nonlinear adaptive criterion
esel,,ename,,182
cm,solid,elem
allsel
nlad,solid,add,box,xyzr,-0.0,9,5,12
nlad,solid,on,,,-2

pred,off
rescontrol,,all,1,20
eresx,no
nlgeom,on
time,1
NSUBST,50,500,5
outres,all,all
solv
fini

说明：上例：/com the 2nd contact paires中的“lmesh,9,12”应为“lmesh,10,12”；