2
\$\begingroup\$

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.

enter image description here

\$\endgroup\$
12
  • \$\begingroup\$ If trace width and spacing are both fixed, the only things you can change to get the right impedance are the distance to the plane below (putting it on a different layer, or using a different PCB thickness) and the PCB material. \$\endgroup\$
    – Hearth
    Jul 20, 2022 at 2:27
  • \$\begingroup\$ What sMMC are you using and why do you feel you need 50 Ω trace impedance for it? \$\endgroup\$
    – brhans
    Jul 20, 2022 at 9:40
  • \$\begingroup\$ Are you sure Altium knows layer 2 is the ground plane? It looks like it's showing two dielectric layers between the signal and ground. \$\endgroup\$
    – The Photon
    Jul 20, 2022 at 14:12
  • \$\begingroup\$ Iirc, for eMMC specifically, the standard package uses 0.5mm BGA, but most of the balls are NC and explicitly allow routing traces through them. So you do not need to trace the signals between the balls. \$\endgroup\$
    – jaskij
    Jul 20, 2022 at 15:13
  • \$\begingroup\$ @brhans: It is in their design guide for the eMMC. \$\endgroup\$
    – Rodo
    Jul 20, 2022 at 20:56

2 Answers 2

1
\$\begingroup\$

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.

\$\endgroup\$
5
\$\begingroup\$

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.

\$\endgroup\$
1
  • \$\begingroup\$ This was useful but the manufacturer confirmed what someone said in the comments. It it is ok to use NC pads for routing. \$\endgroup\$
    – Rodo
    Jul 26, 2022 at 17:07

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.