PCIE branching not detecting PCIe device
Having looked at the board file you posted, the issue is quite clear, you need to basically start again. I'm afraid this answer is going to sound quite blunt.

The main issue that is immediately obvious - none of your PCIe traces are routed differentially. This is the major problem, and shows a fundamental lack of knowledge in high frequency routing.

Once you hit the multi-GHz frequencies that PCIe runs at, you are no longer in a situation where you can just route traces wherever you want and expect things to work. Instead you need to go about the design from the understanding that you are trying to guide radio-frequency signals through waveguides on your PCB.

When it comes to routing high frequency differential pairs you must:


Route Differentially - the P and N traces must follow each others every move.
Match Impedance - traces at RF frequencies act as waveguides with a characteristic impedance. Properly routed traces will have a constant impedance across their length. This should be ~100Ohm for PCIe.
Match Phase - when a differential trace goes around a bend, the trace on the inside covers less distance. Phase matching at the corners basically adds a small deviation to the inner trace to ensure both travel the same distance, and the traces stay in anti-phase.
Separate different pairs - if you run two differential pairs too close together, they will couple on to each other, affecting the impedance and causing problematic crosstalk. As a rule of thumb, inter-pair spacing (separation of different pairs) should be no less twice the intra-pair spacing (separation of P and N) 
Minimise stubs and splits - every time you have a stub or a split in a transmission line, you change the characteristic impedance, and you end up with reflections (like echos) that destroy the integrity of your signal.
Minimise vias - each time the trace goes through the board it causes an impedance mismatch and signal attenuation. For high frequencies you need to minimise the number of vias, and for very high frequencies design impedance matched vias.


You have don't appear to have made any of these provisions in your design. As a result the board is basically useless.

In terms of trying to use resistors in the way you have to isolate pairs, well it is possible, but requires careful planning and design to minimise the resulting trace stubs. You would actually need two sets of resistors at the point where a pair splits to select which of the two paths the signals can go down. You can get away with this approach for Gen 1 and maybe Gen 2 if you are lucky.

However at high frequencies (especially PCIe Gen 3), you'd be far better off using dedicated PCIe multiplexers. These are components which simply act as SPDT switches, but with carefully matched differential and high speed characteristics. You then use a logic signal to select which of the two paths a signal can go down (or come from).

TL;DR; Read up an high-frequency differential routing, and start the board from scratch.