Question about wiring up a ethernet passthrough on my PCB and GND plane(s).

[MostroW]

Hello dear people,

Like the topic header implies i am trying to implement a passthrough for ethernet on my PCB.
Can i wire the connectors pin to pin, e.g. 1 => 1, 2 => 2, etc., or do i have to wire it up according to the 568b specification?

I am totally new to the whole pcb design and as such my current pcb is an ammalgation of three designs, which two schematics i have copied into this design.

Also i am using a 4 layer pcb where layer 2 and 3 are being used in a lattice struct for supplying power around the board and to supply GND, would it be wise to still add a GND copper pour to certain layers or not?

If anyone is interested i could potentially link the design(s) i think as i am using EasyEDA for this.

Any advice regarding the matter would be greatly appreciated, and thank you for your time reading this.

[robertferanec]

Can i wire the connectors pin to pin, e.g. 1 => 1, 2 => 2, etc.,

The best is to imagine how signals are ordered in the coming cable and then imagine if you still will have the same ordering on the cable coming out from your board. Jus follow one wire through cable - connector - pcb - connector - cable and see if it is ok.

For your second question, maybe I would recommend to watch this video: How to Decide on Your PCB Layer Ordering, Pouring and Stackup (with Rick Hartley) https://youtu.be/52fxuRGifLU

[MostroW]

Thank you for you reply mr. Feranec.

The best is to imagine how signals are ordered in the coming cable and then imagine if you still will have the same ordering on the cable coming out from your board. Jus follow one wire through cable - connector - pcb - connector - cable and see if it is ok.

I have a quick test pcb with a RJ45 connector that feeds into a female header, i will use this with some jumper wires to see if my idea about it is correct.
Also i reread my first question saying it's a passthrough where maybe saying it's a coupler to be more exact.

For your second question, maybe I would recommend to watch this video: How to Decide on Your PCB Layer Ordering, Pouring and Stackup (with Rick Hartley) https://youtu.be/52fxuRGifLU

I've watched it and from what i've gathered from it that there is no "one stackup to rule them all" (unless i'm mistaken ofcourse), and the stackup could be dependant on what types of components were used and how high frequency the signal was.

My current situation is a 4 layer board where a good 95% of the signals reside on the top layer and 5% on the bottom.
Layer 2 and 3 are being used with via's to couple GND, 5v, 3v3 to spaces where they need to go, i am currently using a lattice struct where on layer 2 tracks are connected vertically and on layer 3 tracks are connected horizontally through said via's.

3v3 and 5v are always close to GND and the tracks are 1mm wide, but i find myself now in a state confused whether i wouldn't be better off using copper pour on layer 2 and 3 and make it GND?

Would it be bad if i actually poured a GND plane on all layers now i wonder?

[robertferanec]

I am not sure about your design as you write "95% signals are on the top" and then you say "on layer 2 and 3 are tracks". Do you mean power tracks?

If you have 95% of signals on top, maybe I would make L2 solid GND plane, L3 powers and L4 5% of connections.

[MostroW]

I am not sure about your design as you write "95% signals are on the top" and then you say "on layer 2 and 3 are tracks". Do you mean power tracks?

That is correct, layer 2 and 3 contain GND tracks, a 3v3 track and a 5v track, currently it has been set up that layer 2 contains the vertical tracks and layer the horizontal tracks which made they layout a bit easier for me.

I've attached a PNG where you can see the inner 1 (layer 2, brownish color) and inner 2 (layer 3, green color)

If you have 95% of signals on top, maybe I would make L2 solid GND plane, L3 powers and L4 5% of connections.

If my current setup is bad or undesirable then i could backup the current design and try to redraw the power tracks on layer 3 and set layer 2 to a GND plane, if that would produce the desired result(s).

[robertferanec]

You may want to update the PCB. As it is now, it may not be the best layout. You really would like to have solid GND under signals, you may want to follow required impedance and you may want to keep proper distances between tracks (distance/gap required to meet differential pair impedance and also distance between tracks to minimize crosstalk). I would recommend you to watch this video: Understanding Crosstalk in PCB Layout - You may wish you knew this before (with Eric Bogatin) https://youtu.be/5EeQPxRdurk

PS: this really may need to be improved:

[MostroW]

Thank you for your advice, and i've watched the youtube video and also the one that came before that explaining the cross talk itself with the flash example detailing what happens.

I will have a look and see if i can find detailed suggestions on implementing the hdmi connectors in a way that will yield the desired results.

If i would rearrange the power signals to layer 3 would i just cover the whole of layer 2 in one solid ground plane?

[robertferanec]

yes, you may want to have the whole L2 to be one solid GND plane

[MostroW]

I have rearranged the layers and signal and have made some progress though a few things were still confusing.
Using the impedance calculator for the 4 layer stackup at jlcpcb it recommended me a 7628 stackup and to use 8.08 mil traces with 8 mil spacing, but my spacing is 0.5mm do i need to put the tracks closer together to bring it to 8 mils (0.2032mm) to achieve the 100 ohm differential impedance or can i leave that the way it is?

I wanted to download the hyperlynx software to see if i could simulate this, but it seems the free edition has been snuffed out by Siemens which have seemingly absorbed mentor graphics and are not supporting the free edition anymore, which also means they have removed the download option for it, which is a real shame.

Also i have read that through hole components can have some bounce in the signal if you do not route / connect the trace at the bottom of the pin, is this absolutely critical or does this only apply for certain designs?

[robertferanec]

- impedance: I would recommend to search about the topic on internet, but simple answer is, yes, if your signal needs to follow specific impedance, then yes, you may want to use recommended / calculated track width and gap.

- about layout on your board: it still can be improved a lot. If we for example talk about HDMI, that signals are often routed by 100OHM differential pair impedance and you really would like to keep space between the pairs. Sometimes you may also do length matching. I am not sure, but maybe there are HDMI connectors which may have reversed pinout (that could help a lot, you could maybe use direct connection)?

- bounce signal on through hole pins: I am working on a video about this topic, but simply to say, for signals below 2.5GHz you may not need to worry about that

[MostroW]

After reading a bit on impedance and consulting the calculator on the pcb manufacturers website i've adjusted design accordingly, HDMI was calculated for 100ohms and USB was calculated for 90ohms.

I've looked for reverse connection hdmi and rj45 connectors and could not find them on their suppliers website.

My test coupler pcb's came in and i've tested it from module to module using jumper cables and both rj45 and hdmi worked fine, rj45 operated on the same speeds as a normal cable for me, though HDMI i could not test for signal integrity because of missing equipment ofcourse, though it displayed a 1080p image perfectly and no distortion / warping or sound issues.
As both connectors have a shield pin between each pair, should i route the shield connection to the back of the connector or just leave it as it is?
Seeing the test pcb's didn't show any issues with a straight through connection.

Also would it be wise to cover both the top and bottom layer with copper pour connected to ground or would i introduce only new issues with this idea?

[robertferanec]

As both connectors have a shield pin between each pair, should i route the shield connection to the back of the connector or just leave it as it is?

- if you mean HDMI, these are actually GND pins and need to be connected to ground

Also would it be wise to cover both the top and bottom layer with copper pour connected to ground or would i introduce only new issues with this idea?

- I do not normally pour GND on signal layers if I have a solid GND plane in the stackup

[MostroW]

if you mean HDMI, these are actually GND pins and need to be connected to ground

I was a little unsure about that part, looking at some example boards on easyeda and it worked for my testing boards though in the coupler it makes sense it just connects ground to ground.
I will adjust the layout so that the shield connectors go directly to the ground plane on the backside, this will allow me to move the tmds + and - channels closer together for the impedance check.

I do not normally pour GND on signal layers if I have a solid GND plane in the stackup

Would there be any negative impact if one would actually do this?
I could imagine this having effect on the impedance possibly, would it actually throw the impedance off?

[robertferanec]

Would there be any negative impact if one would actually do this?
I could imagine this having effect on the impedance possibly, would it actually throw the impedance off?

Yes, it could have negative impact if not done properly (e.g. unnecessary antennas could be created). Yes, it could influence impedance.