16 January 2018
- Last edited 16 January 2018
What is the goal of your simulation? When I perform a simulation, it is usually to predict the load at which failure would occur, and compare that with the expected service load to calculate a factor of safety. With that goal, I don't need to simulate the behavior of the system beyond the point of failure. That is why a Static Structural model is sufficient to predict the factor of safety. You are not going to see the concrete fracture in the simulation, and the load on the rebar suddenly drop to zero like you see in the physical test because the model doesn't include the ability to simulate element failure, but that is acceptable if your goal is to predict if the design is safe and will be far from failing under the design loads.
I may need nonlinear properties like plasticity in a model, because failure may be defined as collapse, while a test may permanently bend the structure but a small deformation is permitted since it is not a collapse. For this goal, Static Structural is a good tool. Rarely do I want to predict the behavior after failure, but when I do, Explicit Dynamics may be required to simulate element failure and removal from the model during the post failure simulation of the collapse, or in your case, fracture of the concrete.
If your goal is to predict the load at which failure would occur, then I would expect you would plot the Maximum Principal Stress in the concrete, but you have no result for that. Since concrete is a brittle material you would check when the Maximum Principal Stress exceeds the Tensile Ultimate Strength and the Minimum Principle Stress magnitude exceeds the Compressive Ultimate Strength.
I perform a mesh refinement study manually. I solve the model, get a result, make the elements smaller, solve the model, get a result and repeat this until the result doesn't change very much. The result I am tracking is usually stress. Here is one post on the topic. Here is another example. I see you have added Adaptive Mesh Refinement to your solution, which can be an automated way to accomplish a mesh refinement study. I haven't used that before, so I was glad to see it in your model. However, you selected maximum displacement to converge on, and that always occurs on the face of the rebar where you put the displacement load. That defeats the purpose of the Adaptive Mesh Refinement. You want Maximum Principal Stress to be the quantity to converge on.
In your model, you are requesting stress in the same face of the rebar that you are applying the displacement. That is never a good idea. Important results in the model should not be occurring near an applied boundary condition. If you request the stress in the body of the rebar, you will find it is much higher elsewhere, like where it is in contact with the concrete. You are only requesting Normal stress in the rebar. If you want the average stress, you know the diameter and area and have the Force Reaction, so you can calculate the average normal stress by dividing the force by the area.
In your geometry, you have three solids in one component for the concrete, and Topology is set to Share. That means the nodes on the shared face will be common and that is like there is just one big block with deep holes and rebar cast around the center portion. Is that the physical sample, or is the physical sample three pieces of concrete? If it is really one big block, you probably don't need such a large block since the failure will occur in a very small volume near the center.
Another observation is that the rebar is axisymmetric and so is your load and support. That means you could build this as an axisymmetric model and save a lot of time solving.