SimScale CAE Forum

Nonlinear pipe bending test issue

Hello everyone,

I am currently working on this project.

Basicly it is 1/4 a polyethylene corrugated pipe and i want to see the behaviour in large deformations. Also during tests i have deformation in square profile top of pipe. I want see as well but not at first sight.

I dont have yet plasticity spesification of PE, until this i am doing it as aliminum pipe.

My main problem is, i always have “singular matrix problem”. Probably have some problems in contact setup or boundary descriptions but somehow i could not figure it out.

Thank you!!

1 Like

Hey @esavli!

We will check this out and get back to you as soon as we figured out a solution. Obligatory tagging my colleagues, the one and only @fea_squad here that might jump in here in the meantime.

Keeping you up-to-date.


1 Like

Hi @esavli,

I made this copy to the project:

Here is a list of the changes I made in order to make it work:

  • Mesh: second to first order, as it is more stable for physical contacts.
  • Mesh: refined blocks for more precise contact.
  • Imposed displacement and fixed condition: changed from the whole body to external face only. This can be conflicting as causes two conditions on contact faces.
  • Removed blocks from symmetries, as they already have imposed displacement.
  • Individualized physical contacts, switched master/slaves, changed solution method to Newton
  • Simulation control: changed number of cores to 8, as the mesh has 33k nodes.

Please review and post if you need more help.


I think the problem is not the mesh, it’s the boundary conditions,
I have changed the symmetries by manual symmetries (in two directions unconstrained) and chosen a bigger machine and has calculated well without problems.

When we have perpendicular and adjacent faces of boundary conditions , the code can generate problems because you have 2 bondarys in 1 edge, but it is solved making the manual symmetry (Is a classical problem of code_aster and FEA but not difficult to avoid)

great project @esavli , i wanna seeyour resoults :slight_smile:

My changes in


Hi @ggiraldo

Thanks a lot for the configuration. Actually i was trying different combinations so it was messed up :). But many thanks to you it seems really robust now. And i have tried the model with larger displacement and also with plasticity effects and it worked well. Quick question : Can you explain please the switching master/slave thing?

Now i have the next step that meterial behaviour part;

As i said my goal is modeling the polyethylene corrugated pipe and it needed to be modeled as linear viscoelastic or viscoelastic-plastic behaviour. As far as i see we dont have option in Simscale? I have some emprical equations from the literature, How can i use them here to see the required behaviour?

Can you help about this?

1 Like

Hi @camilomati

Thanks a lot for the response and the setup. Manual symmetry is quiet elegant solution indeed. But as i told, during trials some of other configurations was messed up. But it works slower than @ggiraldo solution. Also i compared both solutions with same BC, @ggiraldo model was more robust and seemed true, although need for a validation for sure.


You are welcome!

It is a nice project that you have here, expect to see it finished with some explanation of the results.

Answering your questions:

It might not be totally obligatory, but I think that a contact per pair of faces is more robust. At least that is what I always try to achieve when possible. I had to switch master/slaves because you can’t have one face as slave in more than one contact definition. Physically this makes no difference, only in the algorithm.

Currently the platform supports linear-plastic (with multi-linear curve definition) and hyperelastic coefficient based models (Mooney Rivlin, Neo Hooke and Signorini). If you post your material data/equations we can evaluate if any of this models is appropriate for your case.

1 Like