Simulation of dielectric elastomer with ABAQUS

介电高弹体数值模拟,ABAQUS,有限元模拟

Finite element for the dielectric elastomer. 

When I studied the dielectric elastic, there are not so many ways to simulate the dielectric elastomer. The only way to do it is using a UMAT[1] which is written by Xuanhe Zhao [1]. However, it is not easy to reprogram it, especially since the hyperelastic model is complex, for example, the Gent model. Of course, there is a lot of ways to solve this problem. But it is so difficult for entry-level research who is not familiar with the numerical program. In 2014, I started to know the problem: wrinkle of dielectric elastomer. I have tried with Xuanhe’s UMAT, but it does not work well. I also reprogram it with the Mooney-Rivlin model, but still not work well with my wrinkle problem. I think it is because of the large strain of the dielectric elastomer. And As in the UMAT, I need to build the Jacobian matrix (DDSDDE) which is very difficult.

Then Wei hong introduces a method using a new subroutine called UANISOHYPER_INV, which is very easy to program and can be easily programmed with different hyperelastic models, also using the build-in function of ABAQUS. All the theoretical background is provided in our paper [3]. In the paper, we did not show the details, here, I would describe a little bit how to use this method.

1. Create a material, but don’t add anything

2. Model-\textgreater Edit Keywords
Find the material you just defined. “Add After” *Material, name=…
Add the following 2 lines:

*ANISOTROPIC HYPERELASTIC, USER, FORMULATION=INVARIANT, TYPE=INCOMPRESSIBLE, LOCAL DIRECTIONS=1, PROPERTIES=3

20.62e3,3.983e-11,220

The second line defines two material parameters, the modulus, and the nominal electric field (voltage/original thickness). This example is for gent model that shear modulus=20.62e3, permittivity= 3.983e-11, stretch limit (J), 220

3. Create a section, a part … and all regular stuff

4. Model-\textgreater Edit Keywords Find the part of EAP, Add the following 3 lines before *Element, type=…

*ORIENTATION, NAME=FIELD, LOCAL DIRECTIONS=1

1, 0, 0, 1, 1, 0

3,0

0, 0, 1

This defines a local coordinate system: x in the 100 direction, y in the 010 direction, and 0 rotation (second line)
The last line means the electric field is applied in the z-direction of the local system.
for cylindric system we should define the z-axis

*ORIENTATION, NAME=FIELD, system=cylindrical,LOCAL DIRECTIONS=1

0, 0, 0, 0, 1, 0

3,0

0, 0, 1

5. Find the section you created, add the following keyword to the same line of *Solid Section, …
orientation=FIELD
This would assign the direction defined in step 4 to this section

6. Create a job and add the Fortran file as the user subroutine

 

Please cite our paper [3], if you would like to use this method.

Reference.
1. UMAT is a subroutine in ABAQUS
2. Zhao, X., and Suo, Z., 2008, “Method to analyze programmable deformation of dielectric elastomer layers,” Applied Physics Letters, 93(25), p. 251902.
3. Mao, G., Hong, W., Kaltenbrunner, M., and Qu, S. (May 19, 2021). “A numerical approach based on finite element method for the wrinkling analysis of dielectric elastomer membranes.” ASME. J. Appl. Mech. doi: https://doi.org/10.1115/1.4051212

code: the first zip file is the subroutine (UANISOHYPER_INV) for the Mooney-Rivlin model, also an input file is added as an example. The second zip file is the subroutine (UANISOHYPER_INV ) for the Gent model and the neo_Hookean model.

Files: 

Simulation of dielectric elastomer with ABAQUS》有1个想法

发表评论

您的电子邮箱地址不会被公开。 必填项已用*标注

9  +  1  =  

此站点使用Akismet来减少垃圾评论。了解我们如何处理您的评论数据