Engineers new to Static Structural simulations build a model, overload it and some expect to see the failure appear as a crack in the model. ANSYS has sophisticated capabilities to compute cracks in the model, but this is unnecessary if the goal of the analysis is to see when and where the part will fail.
Engineers learn to compare the state of stress with values provided by a failure theory to decide if the part has failed. This is done by comparing a maximum stress in the model with some limiting value. For example, if the material is ductile, a quick linear elastic analysis will calculate a von Mises Equivalent Stress that can be compared with the Tensile Ultimate Strength. If the maximum stress is larger than the strength, the conclusion is that the part would have fractured. A common method to show failure in a linear elastic model is to set the threshold for the last bar on the legend, which is red, equal to the Tensile Ultimate Strength. If red appears on the contour plot of Equivalent Stress, then it is easy to say that the part has failed under this load and where the part would crack. But people still want to see the crack.
One way to show the crack without using Explicit Dynamics is to use the APDL command ekill. This command removes the element from the model when it reaches the failure criterion; the trick is how to get the model to continue solving after removing the element and incrementing the load.
SimuTech Group, a Premier ANSYS Partner, provided me with an APDL script and permission to share it with anyone. The script implements ekill in a way that allows elements to be removed and the solution to continue. It works best with displacement loads, not force loads. I was successful following the directions to use the script on one model and then another. I release this script into the community, as is, with no support and no warranty. I hope someone else finds it useful.
To show the script in use, I created a 2D plane stress model so each solve would be very fast. The model is a hook with an end load. The question is how much load can the hook support without failure.
I have three systems: Linear Elastic, Elastic Perfectly Plastic and Ekill Script.
In the Linear Elastic model, the legend has been configured so the color red shows elements that are above the Tensile Ultimate Strength of 640 MPa
ANSYS provides a stress tool to make a Safety Factor plot that divides the Tensile Ultimate Strength by the von Mises Equivalent Stress at each node. Therefore when SF < 1 the part has failed, and when SF > 1 the part has not failed.
In the Elastic Perfectly Plastic model, Bilinear Kinematic Hardening plasticity has been added to the Structural Steel model using the Yield Stress that was defined for that material and setting the Tangent Modulus to zero. During the solution, any element that exceeds the yield stress will plastically deform. This behavior can go on way past the point when the material would have failed. If you keep pulling, the element will keep stretching until the shape collapses on itself and the solver will stop because the element has become invalid.
In the plot below, the strain is over 50%, way past the point of fracture.
In the Ekill Script model, the analysis settings are configured with a large End Time of 500 seconds. That means after each one second increment of time, the script will find any elements that have exceeded the strain threshold, remove them from the model using ekill, then submit the job to solve for the next second.
The above sequence is what some Engineers want to see.
The attached project archive for ANSYS 19.0 has the three systems described.