2
\$\begingroup\$

I'm a hobbiest & I've put together a simple PoE board using a LinkIt Smart Duo, the AG9050-2BR and a Bel Fuse 0813-1X1T-57-F. The power circuit works but the Ethernet signal wont work.

The LinkIt has a PHY ethernet output and can be hooked up via traces to a RJ45 Jack. I have tested the LinkIt on its breakout that the Ethernet circuit is working.

Schematic: Simple POE Schematic The AG9050 is not pictured here.

PCB Layout: enter image description here Ethernet Traces are these four just here ^^^^

I've read through this website on tips regarding Ethernet traces. I wish I had done my research prior to getting the board cut. I'd like to know if it is just a trace length/coupling issue or if there are other issues at play.

What do I need to do to ensure the integrity of the ethernet signals on a PCB?

\$\endgroup\$
  • \$\begingroup\$ I can not find reference schematic for network part of the chip, are you sure you properly connected circuit based on 49.9 Ohm resistors? \$\endgroup\$ – Anonymous Mar 23 '17 at 6:07
  • \$\begingroup\$ What do your signals look like? Do you get "fast link pulses"? Can you make it work by forcing both ends to 10mbit? \$\endgroup\$ – pjc50 Mar 23 '17 at 12:20
1
\$\begingroup\$

It depends on the frequency you want to run through the trace, which will depend on if you are running 10Mbit, 100Mbit or 1000Mbit.

Since this uses a 10/100 Phy (the chip that has PHYisical transcievers to drive the ethernet line) if you want to run at 100Mbit, you will need to pay attention to the routing. Ethernet lines ran on the PCB are differential microstrip traces which are a class of transmission lines, so the impedance of the line needs to be matched to the source and the load (the transformer and phy).

Since the mediatek phy doesn't have any reccomendations, these should be a good fit:

From PCB Layout for the Ethernet PHY Interface

PCB Layout Recommendations

  • Keep the traces between the magnetic module and the RJ-45 jack as short as possible — their length should be less than 25 mm (1 inch), and their impedance should be kept below 50 Ω. No vias or layer changes are allowed. A module that integrates the RJ-45 jack with the magnetic module is preferred.
  • The Tx+/Tx- and Rx+/Rx- traces should always be as short as possible (less than 25 mm or 1"). If longer traces are absolutely required, the maximum length is limited to 75 mm (3"). The individual trace impedance of Tx+/Tx- and Rx+/Rx- must be kept below 50 Ω, and the differential characteristic impedance of the pair must be 100 Ω.
  • Route each Tx+/Tx- and Rx+/Rx- pair together, keeping their separation under 0.25 mm (0.01"), using 0.25 mm (0.01") traces. Keep the Tx+/Tx- and Rx+/Rx- trace lengths as equal as possible.
  • The separation between the Tx+/Tx- and the Rx+/Rx- differential pairs must be at least 0.5 mm (0.02"). It is best to separate them with a ground plane.
  • Avoid any off-board wire assemblies. If wire assemblies are needed, use a twisted pair to connect Tx+/Tx- and Rx+/Rx-, and keep their length as short as possible., no more than 75 mm (3").
  • Never use right-angle traces — use 45° angles or curves in traces.
  • Trace widths should not vary.
  • Use precision components (1 percent or better) in the line-termination circuitry.
  • Ensure that the power supply is well regulated (3.3 V DC ±5%).

From the look of it, the board pictured does not have matched lines or differential traces. I would think that this might work for 10BaseT since its frequency requirements are lower, but that is just a guess.

\$\endgroup\$
0
\$\begingroup\$

I am convinced that you have wrong circuit made of R1-R4 and C2/C3. Most probably it should look like like shown on the figure 1 here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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