Elastic Plastic Analysis

[struclearner]

When the loadings causes stresses in the Elastic Plastic analysis higher than the stresses in stress strain curve used, does the analysis continuous until the full load is applied and how the results are then validated.

Thanks for the input.

 

[Erik Panos Kostson]

A simple example that will highlight what is/might be happening.

Plane stress with a plate with a hole. Applied stress on right edge is 100 MPa, and with the stress concentration factor of about 3, the stress at the hole should be about 3 times that. The material is elastic perfectly plastic with 200 MPa yield stress (YS), and zero hardening or post yield modulus (Et=0)

Now the stresses should be capped at 200 MPa. If we though look at averaged nodal results, that is the stresses that are extrapolated and averaged from the solver stress points (Gauss points, GP), then stresses can go above 200 MPa (see left image below), since a difference in stresses between the GP, leads to the fact that when we extrapolate it can go beyond the YS.

If we now look at the raw GP results (using a command before the solution and at the static structural level: ERESX, NO) then as expected the GP are exactly below or at 200 MPa (see right image below), since the material nonlinear behaviour is enforced there (at GP).

Hope this helps explain why one might see higher stresses above yield when averaging to nodes. Of course another reason is that the post yield modulus will give rise to higher stress for higher plastic strains. In this example it is set to zero so it will always be 200 MPa.


Of course if one looks (assuming that the curve has been assigned to the part, and nonlinear material is set) at the von Mises (VM) and equivalent total strain (ETS) at a point, that (VM,ETS) combination/point should be then on the stress strain curve (VM,ETS).

 

[struclearner]

Hello Erik,
Thanks for your reply and clarification.
That is true that after the yielding, the stresses do not rise much but strains do. In FEA, what will cause the yielding of the whole section, I have a model with about 10% of the section is going into yielding and the solution stopped at the final point of stress strain curve with out applying the full load, if I need to determine/approximate, how much load will cause the whole section yielding, we might need to add additional points on the stress strain curve, or is there any other way to figure out the loading causing the whole section yielding.

Thanks for the input.

 

[Erik Panos Kostson]

Normally to determine the plastic moment one can apply a high load which will make sure that it creates a plastic hinge. FEA software will very often then (at least Strand7 which I use) extrapolate the last two points of the stress strain curve if the strains are going outside the curve defined, so not sure what is happening there. Just apply a higher load, but if it will converge that is another question. It might also be that it stops because it fails to converge.

As for analytical solutions there are some basic equations to calculate plastic moments for simple beams and loads. See my last post in:Link ,which is about calculating the plastic moment on a pinned beam (point force load). As I use Strand7, I have the option to use and tweak the arc length method to capture the formation of the plastic hinge (I assume ANSYS to do it in a similar way, but I am not sure). As you will see the agreement is good, so it is possible to calculate that with FEA using beams, or shell/plate elements (and 3D elements of course). Arc length helps here a lot, because we might get a zero or negative stiffness, which load scaling (sub stepping method) cannot deal with.

Hope all this helps.