The fibers are beam elements wrapped on the outside of the solid and you use bonded contact to connect beam, shell and solid elements together.
Under Analysis Settings, your Initial Time Step is too large and you get two bisections before the solver make progress. Change the Initial Time step to 1e-2 to avoid wasting time at the beginning. That doesn't help the solver get any further than you have already.
On the Solution Information folder, set the Newton-Raphson Residuals number of plots to 5 so you can see where the solver is having problems converging. Once you do that, Solve. Now you will have a series of plots under the Solution Information folder to guide you where the model needs improvement. Below is the plot.
The solver cannot achieve equilibrium due to the force imbalance in the model at this location. One corrective action is to use smaller elements. Try that next. It might not let the model get much further.
The beam elements have a linear elastic, isotropic material property so as it tries to bend, large forces build up to limit the bending. But the real material is Kevlar, which has orthotropic material properties. It is very stiff axially, and very flexible in bending. You might need to create a new material for the beams.
A simple idea is to change the beams to LINK180 elements. These will have a hinge at every node. That way, there will be no bending moment in the fiber, but there will still be tensile loads supported. This is probably a more accurate model of the real structure.
After I only reduced the beam element size, the next problem is with the solid mesh. It is too coarse. I recommend going into DesignModeler and using the Slice tool to slice the two ends off the rubber tube. Then pick the three solids and Form New Part to use Shared Topology. Now you will be able to use a Sweep Mesh on the center part of the tube, and put two hex elements through the wall thickness of the tube. Use Multizone Method on the two ends of the tube and again, make sure to get two hex elements through the wall thickness of the ends.
Keep in mind that this is a very complicated model so you will probably have many convergence errors and need to make many adjustments to the model to make progress. It won't be easy.