如何使用Abaqus輸入隨時間變化的材料屬性，是否需要編寫用戶程序？

01-15

有限元，abaqus ，用戶程序

可以用Field Variable+Amplitude實現，具體看

http://www.eng-tips.com/viewthread.cfm?qid=321293

除了*AMPLITUDE和*FIELD應該放在*STEP下，那個範例還有個錯誤，一個是在*ELASTIC行漏了DEPENDENCIES=1。

在Abaqus中超出定義範圍的插值都是常數。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 **

下面是一個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]曲線（其實也是材料的stress[MPa]-strain curve）

虛線是FV1-位移曲線

*Heading

** Job name: Job-twoelementtest Model name: two-element

** Generated by: Abaqus/CAE 2016.HF3

*Preprint, echo=NO, model=NO, history=NO, contact=NO

** PARTS

*Part, name=Part-3

*Node

1, 11., 0.

2, 21., 0.

3, 21., 10.

4, 11., 10.

5, 11., -10.

6, 21., -10.

*Element, type=CPE4R

1, 1, 2, 3, 4

2, 5, 6, 2, 1

*Nset, nset=_PickedSet8, internal, generate

1, 6, 1

*Elset, elset=_PickedSet8, internal

1, 2

*Nset, nset=Set-1, generate

1, 4, 1

*Elset, elset=Set-1

*Nset, nset=Set-2

1, 2, 5, 6

*Elset, elset=Set-2

** Section: Section-1

*Solid Section, elset=_PickedSet8, material=Material-1

*End Part

** ASSEMBLY

*Assembly, name=Assembly

*Instance, name=Part-3-1, part=Part-3

*End Instance

*End Assembly

** MATERIALS

*Material, name=Material-1

*Elastic, dependencies=1

20000., 0.3, , 0.

40000., 0.2, , 1.

40000., 0.2, , 2.

*initial conditions, type=field, variable=1

part-3-1.set-1, 0.0

** ----------------------------------------------------------------

** STEP: Step-1

*Step, name=Step-1, nlgeom=NO

*Static

20., 20., 0.0002, 20.

*amplitude, name=myamp1

0., 0.0

20., 0.0

*field, variable=1, amplitude=myamp1

part-3-1.set-1, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step

** ----------------------------------------------------------------

** STEP: Step-2

*Step, name=Step-2, nlgeom=NO

*Static

60., 60., 0.0006, 60.

*amplitude, name=myamp2

0., 0.0

60., 1.0

*field, variable=1, amplitude=myamp2

part-3-1.set-1, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step

** ----------------------------------------------------------------

** STEP: Step-3

*Step, name=Step-3, nlgeom=NO

*Static

20., 20., 0.0002, 20.

*amplitude, name=myamp3

0., 1.0

20., 2.0

*field, variable=1, amplitude=myamp3

part-3-1.set-1, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step

** ----------------------------------------------------------------

** STEP: Step-4

*Step, name=Step-4, nlgeom=NO

*Static

20., 20., 0.0002, 20.

*field, variable=1, amplitude=myamp1

part-3-1.set-2, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step

** ----------------------------------------------------------------

** STEP: Step-5

*Step, name=Step-5, nlgeom=NO

*Static

60., 60., 0.0006, 60.

*field, variable=1, amplitude=myamp2

part-3-1.set-2, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step

** ----------------------------------------------------------------

** STEP: Step-6

*Step, name=Step-6, nlgeom=NO

*Static

20., 20., 0.0002, 20.

*field, variable=1, amplitude=myamp3

part-3-1.set-2, 1.0

** OUTPUT REQUESTS

*Restart, write, frequency=0

** FIELD OUTPUT: F-Output-1

*Output, field

*Node Output

CF, RF, U

*Element Output, directions=YES

FV, LE, PE, PEEQ, PEMAG, S

*Contact Output

CDISP, CSTRESS

** HISTORY OUTPUT: H-Output-1

*Output, history, variable=PRESELECT

*End Step