How to define a time dependent modulus of elasticity in abaqus explicit?

[ma.vaziri]

Hi all,
I want to model a material with time dependent modulus of elasticity. I think I should do it with VUSDFLD but I'm beginer to write subroutines. If anyone can help me with change my INP file I would thank.
Regards

 

[FEA way]

Actually, you don’t need subroutines to do this. What’s more it can all be done in CAE:
- in material editor select Elastic behavior, change Number of field variables to 1 and specify Youngs’s modulus and Poisson’s ratio pairs for each value of field variable (set Field 1 as 0,1,2,...).
- define amplitude, type time values in the first column while in the Amplitude column put corresponding values of Field 1 from the previous step (0,1,2,...). So for example this pair: Time=6, Amplitude=2 means that at t=6 Abaqus will use Young’s modulus assigned to Field=2.
- in the Load module select Create Predefined Field, choose analysis step, Other and Field. Select whole model. Leave Field variable number as 1, specify magnitude of 1 and select amplitude created in the previous step.

If you don’t use CAE, here’s keyword version:

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

But it should be *Elastic, dependencies=1

 

[ma.vaziri]

Thank you for reply, but in Load module when I create predefined Field and choose analysis step, there is no option to choose Other and Field. Would you please help me with it?
I should say that my analysis step is dynamic explicit.

 

[FEA way]

In versions older than 2018 this feature is not supported in CAE. If you use Abaqus from before 2018 you will have to edit input file and add *FIELD keyword as described in the previously linked thread.