Rupture simulation of a spring retainer

[FArias]

Hello

I am simulating the push-through test on a spring retainer and I would like to determine the maximal load that I can apply. The idea is, basically, to simulate the rupture of the part under an increasing load.
I have defined the spring retainer material to be bilinear isotropic hardening, using the strain at rupture to determine the tangential modulus. My idea is to apply increasing loads until the von Mises stress at any point is higher than the ultimate tensile stress. However, I am having problems with convergence at loads which result in stresses well under the UTS (although big sections of the retainer are already plastic) which I tried to avoid by reducing the element size. Additionally, I have tried with a modified definition of the material, with a higher tangential modulus. Although this solution worked, I am not too pleased with this "faking" of the material properties.

Any ideas?
Thanks in advance and have a nice weekend!

Fernando

 

[crisb]

Sounds like a problem with convergence when the material gets plastic.
You need much smaller time steps (or whatever your program calls them) when the material becomes plastic. Some solvers are much better than others on this type of problem.
Sometimes applying prescribed displacements can help, although I tend to avoid this if I can. Some programs offer an option of specifying maximum displacements on collapse type problems with a load/displacement algorithm which I find work can very well.

 

[corus]

It depends if faking the material properties means that you have gone from an idealised elastic-plastic material (with zero tangent modulus) to applying some value for the tangent modulus above zero. Both could be considered as faking the properties if you don't have the full stress-strain data, and both could be considered as a good approximation, within reason. As crsib says, applying a fixed displacement will ensure a converged solution and the force you've effectively applied can be obtained from the reaction force at the prescribed displacement, thus giving you the result you required.

corus

 

[FArias]

Thanks for the fast answers!

However, I have figured out that the convergence problem was not in the plastic material but on the contact area between the spring retainer and the tool used to apply the press-through force. Sorry about that

Another question: what do you think of the rupture criteria? Is it correct to consider it breaks once it reaches UTS in a certain point? I had also thought about modelling it with a multilinear isotropic which would have the same first two "lines" as the bilinear described above and a final horizontal line at the UTS, to model that with this stress, it can take any displacement on this point (break).

Regards

 

[crisb]

I think its a reasonable approach, having done the same myself. Be careful though not to mix up true and engineering stresses/strains when viewing the results.

Technically it would be more accurate for the third line to be vertical (down to zero stress) or to include rupture within the material model, but these will make convergence much more difficult at the final stages.

 

[FArias]

Hello again

crisb, what do you mean with true stresses/engineering stresses and not mixing them up? If I can correctly remember, engineering stresses are determined over the undeformed cross-section and true stresses over the deformed one. I suppose that when I plot the stresses, they are engineering stresses, right? Can I obtain the true stresses from ANSYS?

I had also thought about the vertical line in the multilinear model, but discarded it for the expected convergence problems.

Thanks again
Fernando

 

[crisb]

Yes, true stresses are higher than engineering stresses at large values of tensile strain.
I dont know Ansys. I have the option of plotting "FE effective stresses" or "effective stresses" in Adina, and have to plot FE effective stresses if I want to compare results with the material (property) input data. I also like to plot plastic strains on this type of analysis.

 

[EdR]

Maybe I'm missing something or didn't understand the post but comparing the Von Mises stress (which is basically a constant times j2' or the Octahedral shearing stress) to a tensile normal stress seems a bit wrong to me.....Usually you compare normal allowables to normal stresses and shear allowables to shear stresses.......

Ed.R.

 

[FArias]

Hello Ed.R.

comparison of the von Mises stress with the UTS as rupture criterion should be a good approximation for steels. It is something I learnt from my old boss but can not confirm nor demonstrate it. Maybe someone with more experience than I could bring some light here.

Regards

Fernando