Beam-to-Solid-Bar-Slip

[cqf_2232]

The model ran successfully after 300 analysis steps. Thanks again for the optimization of my model.

[STKO Team]

you're welcome

[cqf_2232]

Hello, by consulting relevant books, the cohesive force failure first occurs at the loading end, and pull-off cracks appear. After that, the crack gradually developed from the loading end to the free end. However, my model is first damaged on the free end, am I mistaken?

[Horace Horsecollar]

The tau slip is integrated automatically along the bar surface and provides automatically the force-displacement relationship

[cqf_2232]

However, the damage of the model is different from the above-mentioned experimental phenomenon. Why is this?

[STKO Team]

However, the damage of the model is different from the above-mentioned experimental phenomenon. Why is this?

First, you need to make sure all the boundary conditions are correct. I made a guess by looking at the picture you posted, but you need to check it carefully with some details. I imagine you have an article or some report on that.

Then you need to make sure the properties of concrete and the tau-slip law are correct. If you overestimate the tau-slip the damage will concentrate too much on concrete. In the opposite case, the concrete will have no damage.
DO you have some details of the experimental results?

[cqf_2232]

The model I built can be viewed in this article by Murcia-Delso(uploaded), refer to Test No.1 Series No.1, in which the diameter of the steel bar is 36mm, the concrete strength is 34.5MPa, and the bond-slip constitutive reference is CEB-FIP MC90. What surprises me is that concrete with TruncatedDP shows no damage, while DamageTC3D shows damage but low bond strength.

[STKO Team]

What surprises me is that concrete with TruncatedDP shows no damage, while DamageTC3D shows damage but low bond strength

The TruncapedDP shows no damage because you did not set up the optional parameters, and therefore the solid domain is behaving as linear elastic, while all the nonlinearity is given by the multilinear relation you gave at the slip interface.
Of course, it matches the experimental result because that curve was calibrated on that experimental result.

When you use a nonlinear material such as the DamageTC3D, the bond failure will be represented by the concrete itself. What you can do is just use a linear uniaxial material for the slip interface to assign the initial stiffness interface which is lower than the G modules of concrete.

However in this case you will obtain a lower bond strength because in your model the rebar is smooth. The huge amount of bond strength and bond fracture energy, in the experiment, is given by the huge size of the rebar (almost 40 mm diameter) and the relatively large size of the ribs, which propagate the fracture in the concrete as cone shaped micro-fractures, thus increasing the crack-surface size and therfore its fracture energy.

However your rebar is smooth... For this kind of detailed analysis you will either need to model the ribs...
Or...
You can use another concrete model, with a higher fracture energy, in the small zone near the slip

[cqf_2232]

Since the modeling of ribbed steel bars is too complicated, I consider increasing the fracture energy of concrete. Do I need to increase both the tensile fracture energy and the compression fracture energy of the concrete in the bond area? During the modeling process, the concrete needs to be divided into three parts, with the bonding area in the middle. So is the three-part concrete connected with the Merge command?

[STKO Team]

Do I need to increase both the tensile fracture energy and the compression fracture energy of the concrete in the bond area?

Yes, because in a 3D tensorial model (DamageTC3D) the shear behavior is a combination of tensile and compressive behaviors

During the modeling process, the concrete needs to be divided into three parts, with the bonding area in the middle. So is the three-part concrete connected with the Merge command?

Yes, it's important that you use the "Merge" command and not the "Union". Because the merge command keeps the internal faces, that separates the solids from each other, allowing you to assign different materials.

Let us know if you have issues doing it.
However, if you watch the getting-started webinars, we cover the modelling part as well