I'm struggling with a 4 layer PCB (1 signal, 2 GND plane, 3 PWR plane, 4 signal. All Dk=4.3). My boards are usually 2 layers and no impedance control so this is all new stuff for me. I managed so far (using Altium) to setup profiles for a 50 Ω (GPS Antenna) and 90 Ω (USB 2.0 Differential) impedance. While trying to route a eMMC (for data, clk, etc.) I found AN10778, Sect. 4.3. It says that I need 3mils traces and spacing to route the eMMC. I tried to setup another 50 Ω impedance profile but the Altium calculator (picture below) tells me I'm doing something wrong. I tried changing values and Type in the calculator but no luck. What do I need to be able to setup a 50 Ω trace impedance with 3mils width and spacing? Thanks.
I've been told to post my comment as an answer, so here goes.
While eMMC does have a lot of balls, most of them are NC, and usually are safe for routing signals through the pads.
So, if you can route signals through the NC pads, you don't really need fancy vias or thin traces you'd normally need with 0.5mm BGA. You just get the traces going through the pads. The standard pin set up allows you to route the whole thing on a single layer then.
What do I need to be able to setup a 50 Ω trace impedance with 3mils width and spacing? Thanks.
Short of changing board materials, you cannot do that. However, it isn't necessary to impedance match the entire trace as small gaps of different impedance have only a small effect on the signal (so long as the time for the signal to cross them is very short compared to your rise time). Normally what you would do is neck down the trace for a few millimeters to route of the BGA and then switch to your target impedance. As that will result in a discontinuity that takes only a few tens of picoseconds to cross, most likely it will have no effect on your signal.