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
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.
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.
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.