Non linear CCX Analysis - Bilinear isotropic hardening

marco

I don't understand if the plastic behavior bilinear isotropic hardening (with CCX non linear solver an plate elements) is taken into account in the anlysis in tension and in compression.
I am trying to calculate the limit load of a steel plate (yield strength 200Mpa and tangent modulus very small) but in some elements stress in compression is higher -400Mpa (compression).

Thanks,
Marco

Victor

It's probably too coarse a mesh. The yield calculation is done at the integration points inside the elements but the displayed stress is extrapolated to the nodes so it can be higher. Von Mises stress exceeding the yield stress frequently occurs for this reason. If mesh refinement doesn't help, please post a .liml file to help diagnose it.

Andrea

It happens when a node in a element is at the yield and another below. Most of the time the problem is related to constrained nodes and zones where there is stress concentrations but happens also in a element which is far.
If you calculate vMises stress from dat file (which contains stress at the integration points -El Print,S card) you will obtain yield stress. I think that many post processor make a corrections of this.
An idea could be took from Roshaz which has the possibility to interrogate stress at the integration points (selecting an element) and to define a set of yielded elements

marco

Thanks Victor, Andrea for explanations.

Here attached the .liml and the image that show the local concentration (connection between top plate and tube). Like Andrea suggest it is a problem of stress concentration.
I will try with a post processor.

Andrea

Hi Marco!
There are many issue on your model. Hollow section is no properly modelled. In fact plotting with "OUTPUT=2D" parameter activated, is possible to see that nodes of walls are separated (see pictures). Also bottom wall nodes are separated from the plate (are linked only at the corner)

Other problem is the mesh singularity: node athe the iintersection of vertical and horizontal edge of the hollow section creates a singularity and you never reach the convergence of the stress. In other words conducting linear static analysis and reducing the mesh size the stress will increase

Regards

marco

Thanks Andrea for your advice. I made many mistakes, I will improve the model.
Comments in this forum are very useful.
Regards, Marco