I have a different understanding about when failure occurs that contrasts with your statement.
"Determining the location of failure by comparing Total Strain results with the maximum strains defined in the Engineering Data is not so easy,"
For a ductile metal, if we define material failure as the Total Strain when fracture occurs in a tensile test, that has nothing to do with the last value of strain in a multilinear plasticity material model table. The material property that describes the Total Strain when fracture occurs is Elongation. The table of strains in a material model won't have any values of Total Strain larger than the value of Elongation, but the last value in the table might be much less than Elongation. That is okay, ANSYS will continue to solve the model well past the point when Total Strain exceeded the last point in the table. It just won't have any higher value of stress. ANSYS will not stop solving when the Total Strain exceeds the Elongation either. ANSYS will stop solving when the element becomes highly deformed.
That’s why I would like to kill those highly deformed Elements to avoid early convergence issues.
You don't kill elements because they are getting highly deformed, you kill elements because Total Strain is greater than Elongation. If the solution stops due to highly deformed elements and you need it to go further, then you need to improve the mesh, potentially shaping elements that get squashed to a wide-thin aspect ratio at the end of the simulation to be narrow and tall at the start so they have more capacity to deform.
By online help, I mean when you click on the Help menu item and select Mechanical Help.
I created an Engineering Demo (ED) model of a coat hook with a remote displacement that pulls the tip down to demonstrate plasticity and solving past the last point in the material table. I used a Bilinear Kinematic Plasticity model and entered 0 as the Tangent Modulus, to demonstrate what is called an Elastic-Perfectly Plastic (EPP) material. The plastic part of this behavior is just like what happens after the strain exceeds the last point on a multilinear kinematic plasticity material. The video shows what is known as a "plastic hinge".
This model converged to the end. There are some metals with Elongation at break of 100%. The plastic strain at the end in this model is over 200%. This example illustrates the limitation of a nonlinear plasticity model; it is not going to show the tearing of the material when Total Strain exceeds Elongation. To illustrate tearing, the ekill script would be used to remove elements. That is not implemented in this model, but the model is useful as it allows a plot of Total Strain and Pull Force vs. Tip -Y Displacement (up to load step 3).
The hook starts yielding at 308 N. As the tip continues to be pulled down, the force to pull it decreases and the Total Strain increases. Most metal exhibit strain hardening, so the force would increase for some displacement, which is not the case for this EPP material model.
If the material property Elongation at Break is known, then the Tip Displacement where tearing begins could be read from this graph. For example, if Elongation was 0.5, then the Tip Displacement where tearing begins would be 13 mm. If Elongation was 1.0, then the Tip Displacement where tearing begins would be 28 mm. I plan to apply the ekill script to this model and in a later reply, show the result.
Note that this model applies a displacement. If the model had applied a force to the tip of the hook, the solution would have failed to converge after the first couple of increments. The non convergence occurs when the force changes from a positive to a negative slope as the solver would not be able to find an equilibrium after that load.
This EPP material doesn't exist, but if it did, and had an Elongation value < 2.0, then there is an equilibrium for the next load increment, but it is at a 50+ mm deformation and ANSYS can't find something so far away in a Static Structural model. In a physical test, the tip would suddenly drop 50+ mm, but then continue to support higher loads. ANSYS could model this drop in a Transient (or Explicit) Dynamics model.
Attached is an ANSYS 18.2 archive.