以用Field Variable+Amplitude实现,具体看
在Abaqus中超出定义范围的插值都是常数。比如time<86400, FV1=0; time>2.42e+05, FV1=2. 所有插值都是同理。
**
** model level
**
** material definition
*MATERIAL, NAME=myMaterial
*ELASTIC, DEPENDENCIES=1
** E, v, temp, FV1
1.89e+10, 0.3, , 0.0
2.45e+10, 0.3, , 1.0
2.85e+10, 0.3, , 2.0
**
** step level
**
*STEP...
** amplitude to change FV1 during the time
*AMPLITUDE, NAME=myAmp
** time, FV1
86400, 0.0
6040800, 1.0
2.42e+06, 2.0
**
** field variable definition
*FIELD, VARIABLE=1, AMPLITUDE=myAmp
myField-NSET, 1.0
**
下面是一个one element tensile test
**Unit: mm-MPa-N
**
** part level
**
*NODE
1, 0., 0., 0.
2, 1., 0., 0.
3, 1., 1., 0.
4, 0., 1., 0.
5, 0., 0., 1.
6, 1., 0., 1.
7, 1., 1., 1.
8, 0., 1., 1.
*NSET, NSET=N_ALL, GEN
1, 8, 1
*NSET, NSET=N_LEFT
1, 4, 5, 8
*NSET, NSET=N_RIGHT
2, 3, 6, 7
*NSET, NSET=N_BOT_FRONT
1, 2
*NSET, NSET=N_BOT_FRONT_LEFT
1
**
*ELEMENT, TYPE=C3D8
1, 1, 2, 3, 4, 5, 6, 7, 8
*ELSET, ELSET=E_ALL
1
**
*SOLID SECTION, ELSET=E_ALL, MATERIAL=myMat
**
** model level
**
** material definition
*MATERIAL, NAME=myMat
*ELASTIC, TYPE=ISOTROPIC, DEPENDENCIES=1
** E, v, temp, FV1
10e+3, 0.3, , 0.0
30e+3, 0.3, , 1.0
70e+3, 0.3, , 2.0
**
** step level
**
*BOUNDARY
N_LEFT, 1, 1
N_BOT_FRONT, 2, 2
N_BOT_FRONT_LEFT, 3, 3
*INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=1
N_ALL, 0.
**
*STEP
*STATIC
10., 500., 10., 10.
** amplitude to change FV1 during the time
*AMPLITUDE, NAME=myAmp
**time, FV1
0., 0.0
200., 1.0
300., 2.0
**
** field variable definition
*FIELD, VARIABLE=1, AMPLITUDE=myAmp
N_ALL, 1.0
*BOUNDARY
N_RIGHT, 1, 1, 0.01
**
**output
*OUTPUT, FIELD
*NODE OUTPUT
U
*ELEMENT OUTPUT
E, S, FV1
*OUTPUT, HISTORY
*NODE OUTPUT, NSET=N_RIGHT
U1, RF1
*ELEMENT OUTPUT, ELSET=E_ALL
FV1
*END STEP
右面的合力[N]-位移[mm]曲线(其实也是材料的stress[MPa]-strain curve)
虚线是FV1-位移曲线
免责声明:本文系网络转载或改编,未找到原创作者,版权归原作者所有。如涉及版权,请联系删