Building my first multilayer PCB - Improvements and suggestions - Page 1
Forum section: electronics / beginners

author: czbaterka
author_rank: Contributor
timestamp: April 24, 2025, 11:28:13 am
content: Today, I finished my first project for which I will be ordering 2 layer PCB from JLCPCB.It is my first multilayer PCB design and before I order it, I just wanted to check with some folks that have more experience in designing PCBs, what they think, if there is anything I can improve or change to make it better.I already tested the circuit itself on breadboard and it works.This is the schematic for reference:TOP:BOTTOM:What I am little woried about is the GND copper pour. Is very narrow on some places and I am not sure that its enough.Any improvement suggestions?

author: tszaboo
author_rank: Super Contributor
timestamp: April 24, 2025, 11:40:56 am
content: Use vias. Route 95% of everything on the top layer, keep the GND clean and in one piece. Vias are free.You don't have any bypassing capacitors in your design. They are not optional.How are you going to program the microcontroller? Where do you connect the debug probe?

author: czbaterka
author_rank: Contributor
timestamp: April 24, 2025, 11:58:47 am
content: Quote from: tszaboo on April 24, 2025, 11:40:56 amMy original idea was to have digital and low power tracks on top layer and high power, supply and GND on bottom. Should I have just GND on the bottom then? That will complicate the routing quite a bit. Should I for example use vias to "jump" digital track over some supply track?Wym by bypassing capacitors?For programming the MCU, I will use pins that will be added directly to the MCU board. Its an Arduino Pro Mini style board:https://raw.githubusercontent.com/dbuezas/lgt8fx/refs/heads/master/docs/boards/lgt8f328p_pro_mini_qfp32l_pinout.png

author: PGPG
author_rank: Frequent Contributor
timestamp: April 24, 2025, 01:57:11 pm
content: Quote from: czbaterka on April 24, 2025, 11:58:47 amFrom EMC point of view continuous GND plane is crucial.All my 2 layer PCBs are designed that way.My example you can see here:https://forum.kicad.info/t/approaching-pcb-track-routing-for-a-newbie/36302/8All vias you see at this PCB are GND.My strategy is to go with VCC under the microcontroller and then distribute it from there through corners and VCC pins to other ICs.At most of signal lines I use small (47..100 ohm) resistors just to minimize supply current pulses used to charge receiving IC pin capacitance (and track capacitance). Side effect of these resistors is that they help mi to unravel connections.When I have to cross vcc with signal lines I prefer to use 0R than to break continuity of GND plane. I'm probably exaggerating a bit, but 0R doesn't cost much.There are three 0Rs at this PCB. Some other that you can suppose are also 0Rs are ferryte beads I use to connect each IC VCC to main VCC.

author: John Celo
author_rank: Regular Contributor
timestamp: April 24, 2025, 05:05:34 pm
content: Quote from: PGPG on April 24, 2025, 01:57:11 pmHere's one thing I don't understand.If you make a jump over VCC with a 0 ohm resistor you are already breaking up the direct return path underneath with the VCC wire that goes perpendicular/crosses it.Why wouldn't you make that jump using via?What's the difference?Do you have a graphical representation of the path the fields would travel in both scenarious compared?How would it look in a simulation? Does anyone one have a 3d render of such simulation?Does anyone have a drawing of how fields travel in scenarious where resistors "jump" over wires?

author: czbaterka
author_rank: Contributor
timestamp: April 24, 2025, 07:28:52 pm
content: I updated the PCB layout in way that almost everything (what is not GND) runs on top side. Except for few signal wires that I was just not able to put there.Is it better in general that the first version (if you ignore some weird placement of the resistors which I will fix later)?

author: wraper
author_rank: Unknown
timestamp: April 24, 2025, 07:41:46 pm
content: Your "FEEDBACK" may kill the MCU by pushing almost 24V into GPIO. MCU input protection diode won't save it as it will simply lift 5V rail. Not to say it's pointless to have it at all.

author: John Celo
author_rank: Regular Contributor
timestamp: April 24, 2025, 10:40:30 pm
content: I understand what happens if you make a jump with a via and a small, short cut in the 2nd layer ground plane.What I don't understand is what happens in case a resistor is used as a jumper instead.I'm not sure that doing so (using resistor jumper) is better? But can somebody please explain?See picture attached.

author: czbaterka
author_rank: Contributor
timestamp: April 24, 2025, 10:49:20 pm
content: Quote from: wraper on April 24, 2025, 07:41:46 pmHow exactly can the feedback push to 24V? The buffer configuration should never have more on output than its on input right?I actually just wanted to use the second op-amp for something useful (sense the regulated voltage to maybe do slight changes based on load or something).

author: wraper
author_rank: Unknown
timestamp: April 25, 2025, 01:35:40 am
content: Quote from: czbaterka on April 24, 2025, 10:49:20 pmThat's only if assuming that op-amp will always operate gracefully during power on/off, which is not guaranteed.

author: czbaterka
author_rank: Contributor
timestamp: April 25, 2025, 08:23:07 am
content: Quote from: wraper on April 25, 2025, 01:35:40 amSo what do you suggest? Feeding the analog pin directly from the voltage divider? I actually switched to 300k/51k voltage divider (to lower the power losses) so the impedance is relatively high for the analog pin. Maybe like 100nF capacitor on the analog pin would help? I dont need very quick response...

author: PGPG
author_rank: Frequent Contributor
timestamp: April 25, 2025, 02:12:32 pm
content: Quote from: John Celo on April 24, 2025, 05:05:34 pmI'm rather jumping with VCC over signal lines. For example at my picture at top right of main microcontroller. With one 0R I jump over 3 signal lines.Quote from: John Celo on April 24, 2025, 05:05:34 pmImportant is if return current can travel directly under signal track and not if it happens the another wire be between them. What counts is the area surrounded by signal and its return path.It is not such that if return current in GND plane crosses than they collide with each other in any way.Quote from: John Celo on April 24, 2025, 05:05:34 pmReturn current for the track that uses no vias have to go around vias of the second track increasing the area in which that signal travels.Quote from: John Celo on April 24, 2025, 05:05:34 pmI am using only my imagination. Never had access to any field simulation software.I am also very surprised seeing at KiCad forum that people use Spice to simulate big (whole) circuits. I have only used it to see effects of parasitic components of L and C in supply filters. For 'normal' signals I don't see a need to simulate anything - they simply work as they are intended to.Quote from: John Celo on April 24, 2025, 05:05:34 pmIn my imagination the signal traveling through 0R is simply slightly raised above the level of the PCB in this place. It is much less area increasing than by the need to go (for return current) around vias.

author: PGPG
author_rank: Frequent Contributor
timestamp: April 25, 2025, 02:26:34 pm
content: Quote from: John Celo on April 24, 2025, 10:40:30 pmDon't look at voltage field between signal track and GND return path.What cares is the variable magnetic field generated by current flowing in closed circuit. The higher current and the higher area the field will be higher.