Metal tensile testing, loads given as force vs displacement

  • 286 Views
  • Last Post 22 November 2018
obiforeva posted this 22 November 2018

Hi everyone,

I'm trying to figure out element distortion problems in ANSYS. I generally study on fiber reinforced composite materials but for a case study, I did some testing on aluminum pressure vessel. I did burst testing on Al vessel and also, I extracted tensile test coupons from the vessel and done some tensile testing according to ASTM E8 standard.

So I want to model these two cases (internally pressurizing the pressure vessel and tensile test). I started with the simpler case, Al tensile testing. I had the experimental data, so I know the yield Str. and post yield behavior. I used both bilinear and multilinear isotropic hardening models. For multilinear hardening, I entered tabular data which I calculated true stress and strain from experimental engineering stress and strain up to max. eng stress (after that necking begins and conversion equations are not valid). I removed the grips and applied boundary conditions and loads to end faces. 



You can see the results in the figure. I'm using video extension-meter and it measures displacement between two marked regions. I have marked same regions in ANSYS and plotted with external program for comparison.

 



Multilinear hardening fits well if the experimental data were provided. But I realized that, if I apply load as displacement, I can see necking and post-necking behavior of the metal (error margin increases but at least behavior is OK as you can see in the figure). On the contrary, if I apply force rather than a displacement, I get convergence errors after max. stress point (specifically element violations) and so, I cant see any necking or post-necking behavior (red curve in the figure).

I have done some search about giving force as a boundary condition and convergence and I see that it is about calculation method so that force (or stress) should monotonically increase. If there is any decrease, it will stop calculation and give a convergence error.

Can someone give any clarification to this behavior or any work around? (Such as arc length method rather than Newton-Rhapson)

I suspect that similar I'm getting similar convergence problem for determination of burst pressure of Al pressure vessel. Because I'm getting convergence errors after applying internal pressure of 19.7 MPa. But in experiments, burst pressures were around 23.5 MPa. Unfortunately, I can't give displacements as load in pressure vessels. 

I also tried to give multilinear tabular data including post necking true stress and strain using some kind of power law but no change about convergence problem. 

I'm hoping that overcoming this post-necking convergence error will increase my accuracy for determination of burst pressure of metal vessels.

Regards,

Serkan.





Order By: Standard | Newest | Votes
peteroznewman posted this 22 November 2018

Hi Serkan,

Thank you for posting a discussion with a full description of your problem and a clear set questions to answer.  I will answer some of your questions.

I have built tensile test models using these kinds of samples and materials before and I always use displacement input.

I don't use a force input because the solver can only approach the peak of the force-displacement curve. It can't normally go past the peak simply because it gradually increments the force and looks for equilibrium, but there is no equilibrium past the peak on the force-displacement curve.

I understand that with a pressure load, you can't simply switch to displacement the way you can with a tensile test. However, there is a setting that allows the solution to progress. That is called Stabilization. You turn that on under the Analysis Settings menu in the Nonlinear Controls category.

Arc-length methods are also available, but you must insert an APDL command snippet to do that. Look that up in the ANSYS Help system.

Regards,
Peter

  • Liked by
  • obiforeva
SandeepMedikonda posted this 22 November 2018

Serkan,

  To add to what Peter said, I want to point out to 2 specific sections of the help which deal with unstable structures and also convergence in such structures. They highlight a couple of other ways you can try.

Regards,
Sandeep
Guidelines to the Student Community

  • Liked by
  • obiforeva
obiforeva posted this 22 November 2018

Dear Peter and Sandeep,

Thank you for the quick response! These are exactly what I expected as a feedback from this forum. I'll look your suggestions asap and will post updates.

Regards,
Serkan

Close