If you extrapolate the trend, you would predict that the lines will cross and the solution will converge, if only the solver would have kept iterating! Can you think of the place where you told it not to give up until 50 iterations? Why don't you change the number from 50 to 100 and see what happens?
I initially did some work on the wire that goes off at an angle to the side while wrapping around the arc of that link. It seemed to me that the wire is on the verge of sliding off the arc and ending up at the side of the link instead of on top. That kind of sudden change in contact status is toxic to convergence. This is not a good design. The link should be wider at the base so there is no chance that the wire will slide off the edge. Bad designs are harder to simulate than good designs.
To address the need to know the contact stress of the part the wire slides on, I would build a dedicated model just for that. It would be a very simple model like the ones I provided above. I would make it a parametric model that will create any of the wire contacts in the assembly. The parametric inputs are the bend radius, the wrap angle and the tension. Using the Parameter set capabilities of Ansys Workbench, you can copy/paste a spreadsheet with as many rows of inputs as you like, then click the Update All Design Points and Ansys will automatically build each of those models and solve them to report the contact stress. The system model of the entire finger (using springs) computes the wire tension values for any load in any configuration. The system model can also be a parametric model to assemble the links in all configurations of interest. By separating the analysis into two models, each one converges easily. This is a great approach that is a widely used by analysts in many fields.
You are navigating away from the AIS Discovery experience