Creep simulation in ANSYS. APDL Scripting.

Описание: This is how you can simply simulate creep phenomenon in ANSYS. The following APDL code is also helps you to manipulate it to your own model:
------------------------------------------------------------------------------------------------------------------------------------------------------
finish
/clear
/PREP7
!*
ET,1,PLANE182
!ET,1,PLANE183 ! 183 without keyoption
!*
KEYOPT,1,1,1 !!!! K1=0:full integration /// & K1=1: reduced integration
KEYOPT,1,3,0 !!!! (K3=)0:Plane Stress ***
!!!! 1: Plane Stress with thickness ***
!!!! 2:Plane Strain
KEYOPT,1,6,0
!!!!!!!!!!!!! Material Properties (MP)
!!!!!!!!!!!!! MATERIAL 1 = ADHESIVE
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,1,,2232
MPDATA,PRXY,1,,0.4
TB,CREE,1,1,4,2
TBTEMP,0
TBDATA,,0.999235e-6,2.87,-0.4277,0,,
!!!!!!!!!!!!!!!! MODELING
*set,LT,130 !!!! total length
*set,Lg,24 !!!! grip length
*set,Lm,52 !!!! middle length
*set,Hg,20 !!!! grip height
*set,Hm,10 !!!! middle height
*set,Rf,25 !!!! fillet radius
*set,thick, 2 !!!! thickness
RECTNG,0,Lm/2,0,Hm/2,
RECTNG,Lt/2-Lg,Lt/2,0,Hg/2,
LARC,3,8,4,Rf,
L,2,5
lsel,s,loc,x,Lm/2,Lt/2-Lg
al,all
Allsel,all
esize, 1
allsel,all
MSHAPE,0,2D !!!!!!!!!!!!!0:quad, 1:triangular
MSHKEY,1
amesh,all
!!!!!!!!!!!!!!!!!!!
!!!!!!!!!!!!!!!!!!!!! LOADING
!!!!!!!!!!!!!!!!!!!
P=4 !!!!uniform applied load MPa
/sol
nsel,s,loc,x,0
nsel,r,loc,y,0
D,all, , , , , ,UY, , , , ,
nsel,s,loc,x,0
DSYM,SYMM,X, ,
nsel,s,loc,y,0
DSYM,SYMM,y, ,
nsel,s,loc,x,Lt/2
SF,all,PRES,-P
allsel,all
solve
!***************** Creep control
DELTIM,1e-1,1e-3,5
OUTRES,ERASE
OUTRES,ALL,10 !!!!!!!!!!!!!!! Save every N=10 substeps @@@@@@@@@@
RATE,1
TIME,1000 !!!!!!!!!!!!!!!!! creep "TIME" per seconds @@@@@@@@@@@@
SOLVE
save