Generally student posting is disallowed on this forum, but I'll do my best to get you pointed in the right direction.
Okay, well in that case let's start by simplifying the model down to only what is necessary to find a solution. The slider track does not contribute to the solution in any significant way, so you should remove it. The cup that the probe slides into also does not contribute to the force on the spring. There should only be three parts of your model: The slider, the probe, and the spring.
Once you've suppressed the other parts, I'd suggest that you utilize symmetry. Also, you could recognize that the probe will never interact with anything outside of the notch and cut off the slider at the vertical edge of the notch. You will also not need any of the geometry beyond the notch, so you could cut that off as well. Finally, you'll want to bring the surfaces into initial contact; Ansys will have difficulty seeing the initial interaction if you try and simulate them coming into contact... so move the slider such that it is just touching the probe. You can accomplish all of the above geometry manipulations in DesignModeler.
After you've utilized symmetry, truncated the model to a more managable size, and brought the surfaces into initial contact, you should then bring the model back into Ansys Mechanical Simulation and apply your boundary conditions. You'll want to use a Pure Penalty or Augmented Lagrange (slightly more accurate) contact formulation to simulate the interaction between the probe and the slider. You'll probably want to use the "Auto-Axisymmetric" option if you're interested in the contact pressure at the interface, otherwise the results may be difficult to interpret. I'd start with friction turned off, and then turn it on once you get your model to converge.
Before solving the model, be sure to turn on "Auto time stepping". Ansys is using nodal force iteration to determine the interaction at the interface between the probe and the slider. If you take too big of a load step, it may have difficulty converging. Auto time-stepping allows Ansys to automatically bisect the loads until it is able to find a solution (or until it hits the max number of bisections).
Hopefully that gets you pointed in the right direction. Keep an eye on your mesh quality and try to use a brick mesh where possible, as it is more efficient. You should be able to brick mesh this entire model. Let me know if you have any questions.