Orthotropic material simulation not converging - Ansys Workbench

[MicheleB]

Hi all,
I am trying to run a simulation in Ansys Workbench 17.1 in which I have 3 bodies: a flexible body between two rigid bodies. The lower rigid body is fixed and the upper rigid body rotates (applying a joint load) compressing the flexible body in between. I am using two bonded contacts and MPC formulation. Large deflections are on.
Everything works fine when I define a linear elastic isotropic material for the flexible body, but when I try to define an orthotropic material the simulation does not converge, unless my axial and shear modulus are within a certain range.
Anybody has any idea why I am not free to choose the material parameters?
Thanks!

 

[NRP99]

With such limited information of the error and limited knowledge about orthotropic materials, it is difficult to answer this question. But if the error for convergence is rigid body motion then you need to refine your mesh and make it same on the contact and target bodies. Also keep the weak springs option on. The convergence error will define whether it is be due to material parameters of the general convergence issues. You can search online for specific error massage and rectify it by setting some parameters in the contacts, analysis setup and by remeshing.

Mostly it will be due to general convergence issues for isotropic materials but not sure about the orthotropic materials cause never used.

 

[MicheleB]

Thank you for the answer, I'll check those things out.

 

[IceBreakerSours]

The flexible body in between will not only be under compression but also shear and tension, at a minimum. So, the material model must provide those stiffnesses to the solver. Also, you do NOT want to assume linear elasticity if a body is undergoing finite deformation. What you need to assume is either isotropic or anisotropic hyperelasticity (transverse or orthotropic symmetry), depending on how accurately you want to model the tissue under consideration.

It is hard to explain without knowing the background but suffice it to say that you CAN NOT choose material constants at random except in some rare circumstances. Some materials under some circumstances may be assumed to be linear but that happens to be a small set of situations. Chances are you provided constants that the solver got upset about because you are making it do something it finds hard or impossible to do. I suspect ANSYS must have dumped some warning/error messages in solve.out related to the material constants.

Health warning:

If you are interested, strain energy convexity is what you want to read about [Schroeder, Neff, Itskov are some recent scholars in this area]. It is a non-trivial matter, especially if continuum mechanics or math aren't among your strong suits. However, if you have a feel for mechanics, read about Drucker stability criterion. What this criterion says is that incremental work due to incremental load/deformation should always be greater than zero OR the deformation energy in deformation space must be bowl-shaped OR the elastic stiffness tensor must be positive definite OR all eigenvalues of this tensor must be greater than zero. These are all equivalent statements. It specifies a constraint on the choice of the constants, which should suggest to you that not all constants must pass this constraint. Therefore, you can not randomly select material constants in all but a small set of situations.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[MicheleB]

Many thanks for the detailed response