6
\$\begingroup\$

I'm finally dipping my toes into PCB design as I got around to finishing up my schematic for an upcoming project that I'm working on.

If it helps in finding a solution to my problem, this PCB will take a mixed signal approach. If not, please ignore it.

The issue at hand is essentially: how can I deal with rat lines that are crossed over each other? The only solutions I see is jump the trace from the top layer to the bottom layer, or redo the footprint from the IC.

It doesn't matter how many times I rotate or organize other components. The ratlines are always crossed over on each other.

I'm currently using EasyEDA as the schematic and PCB editor using the community's footprint design, so I am not sure if that's where I went wrong.

Be warned. This is my first time attempting a PCB design, so what can I do to improve?

Here's a picture with what I'm dealing with.

Enter image description here

This is not the final product as I'm stuck on the left side of the board where the microcontroller is.

\$\endgroup\$
7
  • 7
    \$\begingroup\$ Why are you worried about the ratlines? Of course they are going to cross - otherwise laying out a pcb would be easy! Use the ratlines as a guide for density and aligning the components, but crosses are inevitable. How is redoing the footprint going to change anything? Engineering is finding a workable compromise. \$\endgroup\$
    – Kartman
    Commented Feb 10, 2021 at 6:38
  • 1
    \$\begingroup\$ @Kartman Oh! Its because when I start the tracing, I cant cross over traces with each other. \$\endgroup\$
    – Leoc
    Commented Feb 10, 2021 at 6:39
  • \$\begingroup\$ I might have figured it out, just saw you can interchange the trace to be top and bottom layer \$\endgroup\$
    – Leoc
    Commented Feb 10, 2021 at 6:41
  • \$\begingroup\$ Are you going to etch these at home, or have them fabbed at a legit shop? \$\endgroup\$
    – The Photon
    Commented Feb 10, 2021 at 6:45
  • 1
    \$\begingroup\$ "The only solutions I see is jump the trace from the top layer to the bottom layer" - Have you looked at any commercial PCB? They are full of these jumpers (called vias) \$\endgroup\$ Commented Feb 11, 2021 at 12:28

3 Answers 3

24
\$\begingroup\$

You can use vias to move a trace from top to bottom and back again. That's like your "jump the trace from top to bottom solution." That's the usual way of handling crossings - make one trace go below the other.

What you really need to do is to move your parts around and rotate them to minimize the number of crossings before you start routing.

  • Use the entire bottom side as ground. Try to keep it in one large piece. Anything you run on the bottom to get around a crossing should be as short as possible.
  • You have audio and fast digital stuff on there. Try to keep the traces for the two types of signals away from one another.
  • Group your parts so as to minimize crossings, even if it offends your sense of organization/aesthetics.
  • Group your parts so as to keep digital stuff and analog stuff separate. When in doubt, keeping analog and digital seperate is more important than minimizing crossings.
  • Use vias to connect all ground connections straight down to the ground plane on the back side.
  • You can pretty much ignore the ground connections until the very end. Route all of your signal lines and power traces, then pour the ground plane on the back. Drop the ground connections to the ground plane with vias.
\$\endgroup\$
6
  • \$\begingroup\$ What an amazing response thank you! I am going to use a 4-layer pcb so the same way you mention of using VIA to GND I am going to do that with PWR and cut the planes up to 5V, 3.3V and 24V. \$\endgroup\$
    – Leoc
    Commented Feb 10, 2021 at 7:01
  • 2
    \$\begingroup\$ Perfect, glad to hear it'll be okay. How would separating (Spacing) a ADC work is that consider Analog, or digital, or even both? Thanks again for the response \$\endgroup\$
    – Leoc
    Commented Feb 10, 2021 at 7:04
  • 7
    \$\begingroup\$ An ADC is both. Try to place it so that it is on the border between "analog land" and "digital land." \$\endgroup\$
    – JRE
    Commented Feb 10, 2021 at 7:12
  • 3
    \$\begingroup\$ You can ignore ground until the end, BUT, try to leave room for ground vias if component placement gets tight. \$\endgroup\$
    – user57037
    Commented Feb 10, 2021 at 8:53
  • 1
    \$\begingroup\$ If you want clean analog, power the audio on a separate power bus from the digital circuits. If you have mixed signal devices, check their specs for how to properly power the two circuit types, if they allow for that, and be careful with power-on sequencing. I was handed a prototype board once that burnt out it's mixed signal SOC device, after ~100 hours of operation, because the analog power rail was able to light up that side of the chip, just a few tens of microseconds before the digital side reached minimum voltage. The bias caused dopants to migrate and created an internal short. \$\endgroup\$
    – jwdonahue
    Commented Feb 10, 2021 at 23:23
2
\$\begingroup\$

One strategy that was more common with older designs is to route traces vertically on one side and horizontally on the other. This method will likely need more vias than if you don't follow this pattern but it keeps things organized and can greatly improve the density of traces you can fit in one area. Here's a picture of a section of a board I designed recently that uses this strategy. Of course this also prevents you from using the bottom as a complete ground plane, makes the lines longer and more inductive, and has other cons too so it's not appropriate for every application, but works nicely for low frequency and low power projects with a lot of connections.

Red (front) traces move vertically. Green (back) traces move horizontally.

Also, as JRE mentioned, arranging elements carefully to minimize trace length makes a world of difference.

\$\endgroup\$
2
  • 3
    \$\begingroup\$ That was an effective strategy for through-hole boards because every pin was a free via that took up zero space. These days it's more like laying out a single-sided board so placement becomes more critical (as does swapping pins that don't matter on things like resistor arrays or using different inverters in the same package to simplify the routing). \$\endgroup\$ Commented Feb 10, 2021 at 20:10
  • \$\begingroup\$ Even though one can't have a complete ground plane when using Manhattan routing on a double-sided board, drawing "grids" of horizontal and vertical power and ground wires that are stitched together at every intersection can minimize the area of current loops, as well as the worst-case "slot size". \$\endgroup\$
    – supercat
    Commented Feb 10, 2021 at 20:12
0
\$\begingroup\$

Zero ohm resistors make handy bridges, so one track can hop over another. Run a track between the pads of the resistor. That's probably best done on whichever track doesn't have a signal that may be degraded by the extra component.

\$\endgroup\$
1
  • 3
    \$\begingroup\$ On a two layer PCB, just use vias to cross to the bottom and back to the top. I think zero ohm resistors (or jumper wires) only make sense if you have a single layer PCB (i.e. because you etch it at home). \$\endgroup\$
    – Michael
    Commented Feb 10, 2021 at 20:29

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.