Tips for transitioning from 2-layer to 4-layer? - Page 1
Forum section: electronics / general

author: smbaker
author_rank: Regular Contributor
timestamp: January 15, 2018, 11:04:16 pm
content: Hello,I'm not a professional, I've done what I consider to be hobbyist-quality work with Eagle. I use Eagle because it's the tool that I know how to use, not because I particularly like it. I do often use the autorouter, even though I know it's frowned on by many. Over the years my projects have ranged from simple to moderately complex 2-layer boards, usually 100mm square or less. I've never considered a 4-layer board under the assumption that it would be cost prohibitive to do so. Checking one of the online quotation sites (Seeed Fusion, which I've been using recently), it shot me a quote for a 4-layer board that's only 11% more than a 2-layer board. That's assuming I used the quotation tool correctly and didn't mess something up... which is always possible.Anyhow, I have a board with about a dozen ICs on it, and it seems like it sure would be convenient to have Vcc and GND on separate layers. It would make the signal layers cleaner not having to deal with the power traces, and it would lead to nice big power and ground planes for all the ICs. I was thinking of just dumping Vcc and GND polygons in the middle, then going about the signal traces like I normally would on the top and bottom. I don't need or want to do anything fancy, no blind vias, no buried vias.What I'm looking for is any tips for making the transition from 2-layer to 4-layer, any pitfalls to avoid, etc.Thanks,Scott

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: January 15, 2018, 11:12:39 pm
content: General first step - put and GND on inner plane layers to clear space on outer layers for routing, then treat as per 2-layer.If you don't need Vcc everywhere and/or it doesn't need to be a plane, and routing on outers is tight, keep gnd as an inner layer plane and second inner as signal layer with VCCWhen you're done see if there's anything on the inner layers that can easily move to outers, for accessibility - track hacking etc.

author: smbaker
author_rank: Regular Contributor
timestamp: January 16, 2018, 01:30:31 am
content: It seems reality has destroyed my hopes of cheap 4-layer PCBs.Turns out it was just abugfeature in Seeed's estimator tool. If I click to change from 2-layer to 4-layer, it resets the board dimensions back to 100mm x 100mm. Fixing the board dimensions, the real price of the quote was approximately double. At some point I might cut my teeth on 4-layer using a smaller design, but not with the board I'm working on this evening.On the positive side, I did manage to learn some new things about Eagle.Scott

author: Siwastaja
author_rank: Super Contributor
timestamp: January 28, 2018, 02:04:20 pm
content: Use pcbshopper.com to find out which one's actually the cheapest. It might be that some of the cheaper ones (such as PCBway) ends up being the same cost for 4-layer you are currently paying for two layers.For prototypes / small batches, I typically dedicate upper mid layer for full ground plane, and bottom layer for power distribution. This leaves top and lower mid for routing.

author: montemcguire
author_rank: Regular Contributor
timestamp: January 31, 2018, 05:05:39 am
content: I use 4 layer a lot for high precision analog, and find it invaluable. Typically, I use the outer layers for routing and ground copper pours. I use the inner layers for + and - power using copper pours, with some routing in these layers, as long as it doesn't slice up the foil too much. I don't often use controlled impedance traces, so I don't need to route over a clean plane, but your circuits may be different. Still, I have successfully laid out a 420MHz current feedback amplifier with some inner layer copper cuts and special keepaway distances for sensitive nodes, and the layout was stable the first time. So, you can do high speed work without a 'perfect' plane as long as you're careful about things.Some of the things to keep in mind for low cost 4 layer are that you have to use vias that go all the way through the PCB for lowest cost. Blind or buried vias would be great, but they're too pricey for me. The clearances on the inner layers are typically larger than for the outer layers, so make sure that you set your DRC parameters for this. I'm using a 7 mil outer layer clearance with a 10 mil inner layer clearance. The inner layer clearance can be set by changing the isolate parameter of the polygon used for the pour on that layer - there's no explicit place in Eagle's DRC rules to set this, but using 7 mil in the clearances section and then using 10 mil in the polygon settings, you can get this to work.I use a 10 mil minimum drill size for low cost, but I often use 15 or 20 mil drills so that they are slightly lower impedance, and are more reliable. The 62 mil stackup is tall compared to a 10 mil drill, so if you don't need a tiny via, why push the fab process that much. But, these larger drills, along with their restring size and clearance, are not able to route 0.5 mm pitch logic, so you sometimes absolutely need a 10 mil drill to handle an 0.5mm pitch SMD part with a logic bus.Overall, the most important thing is to get your Eagle DRC parameters set well, and use design rule check often. It's silly to push the limits all the time, but the 7 mil outer space/trace, 10 mil inner clearance, 7 mil restring, 10 mil minimum drill, and 20 mil copper/dimension clearance seems to work well for Advanced Circuits lower cost process.Best of luck!