Platform forum

USB Controlled Impedance on 4-Layer PCB (routing on L3)

GeorgeIoak , 07-10-2019, 03:49 PM
I'm finishing an open source board which will be a low cost High Speed USB Analyzer. Jumping from 4 layer to 6 layer in low quantities is expensive so I've challenged myself to try and finish the design with 4 layers but also trying to use good design practices. My layer stackup is:

L1: Signal
L2: Ground
L3: Power/Signal
L4: Signal

For a better user experience I want to place the USB connector which connects to the PC on 1 end of the PCB and the USB connector that you plug your device into at the opposite side of the PCB. In this screen capture I've highlighted the USB D+/D- traces which have a length of ~30mm

I plan on using JLCPCB and their layer stackup information can be found here.

I was experimenting with Saturn PCB Design Toolkit and came up with these settings:

I'm not sure if I've used the tool properly so I'd appreciate someone having a 2nd look at this. To make matters worse AD 19.1.5 isn't agreeing with these numbers:

Since I want USB High Speed performance out of this board I'd like to do the best I can while still using the 4-layer PCB. The only other thought I had was to drop all of the top side BGA escapes on the left side down to a lower layer and that would allow me to escape D+/D- on the top layer and route it to the left and up to the micro USB connector. That's a lot of extra effort which I'm not sure is worth it.

Thanks in advance,
robertferanec , 07-15-2019, 01:58 AM
I do not use Altium for impedance calculation, so I am not sure about the numbers there, however, in saturn PCB you need to specify reference planes (you can see reference planes on the picture above and below the trace). The question would be - are you going to have GND solid plane above and below your USB tracks? Because if not, the calculation will not be correct.

What is the chip, is it an FPGA? Is not possible to move the USB BGA pins on the other side of the BGA?

I would simply try to make the USB as short as possible. Maybe, I would consider to have the connectors on one side for hobby project or prototype. For professional product, I would probably make the board as small as possible and used a proper PCB stackup.

PS: Is the schematic finished? E.g. I do not see any protection on USB nor capacitors around USB connectors.
GeorgeIoak , 07-15-2019, 10:32 AM
No, unfortunately I only have a solid ground plane on L2. With so many signals on a 4 layer board I could not keep a solid ground area on L4. This started as just one of those projects that I said "I wonder if this would work" and it kind of snowballed from there. I originally did have the micro USB connector at the bottom edge next to the USB A but looking at it and thinking of how the board would be used I convinced myself to move the micro connector up to the top and see if I could get close enough.

I made some additional changes to try and help routing out all the other signals and I was able to break out all the signals to 1.27mm pitch TH connectors around the edge of the PCB. The 24-bit LCD signals are arranged in order on the left which made things a bit more difficult and added extra vias which turned this into a bit of a mess.

The schematic isn't finished. I've left some room on the bottom of the board and plan on adding a few more things but I wanted to see if I could even come close to a decent layout. It still has a lot of work but here;s what it looks like now:

Lakshmi , 07-16-2019, 06:44 AM
- Try to keep USB Pair signals as short as possible.
- I don't see any ESD near the USB signals nor the Decaps for the Power pins.
- Have you looked into the reference design of the chip?
- I believe one on the bottom USB Connector uses USB-UART (USB-TTL) which you could have moved on to the top and Other USB you should have kept near the USB pin of the BGA.
PS: I'm not sure which BGA chip it is.
GeorgeIoak , 07-16-2019, 12:35 PM
Yes, I've done plenty of USB designs and controlled impedance but this design is a matter of trade-offs and what can be done that is outside the normal design criteria. I was hoping to see if anyone else had any first hand experience to see what's been done before.

The main part is a LPC4357, SDR SDRAM on the right, and a USB3343 on the bottom.
robertferanec , 07-17-2019, 06:05 AM
Possibly, maybe there could be a way to go with the USB on the TOP and route it mostly there (maybe I would try to move some of the top connections to the headers on different layer to make space for the USB). In that case you could use L2 solid GND as the reference plane and it could be more easy to route USB with required impedance.
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?