4-layer PCB -- still use ground fills on front and back? - Page 1
Forum section: electronics / projects

author: ebastler
author_rank: Super Contributor
timestamp: March 27, 2021, 06:38:11 am
content: I am working on a largish 4-layer board (with uninerrupted GND and VCC planes inside, no traces there). What is the recommended practice for the outer layers -- should I still use ground fills there, or leave just the traces?Electrically it seems to me that ground fills are undesirable in this situation: The additional ground areas would increase the trace capacitance. And they should not do much good for reducing crosstalk between traces, since when traces run close to each other there won't be room for the fill anyway. So I am inclined to use no ground fills on the outer layers.Or are they beneficial from the manufacturing process' point of view? I have read somewhere that etching of the traces can be controlled better if they are not left "lonesome" on a large copper-free area; but that might be outdated advice? Just reducing production waste, by asking for less copper to be etched away, is another production-related reason I could see. And avoiding a "copper imbalance" on the two sides of the PCB sheets was also stated somewhere as a reason for fills.So, ground fills or not? Thanks for your advice!Edit: Elaborated on potential manufacturing benefits...

author: Siwastaja
author_rank: Super Contributor
timestamp: March 27, 2021, 08:07:01 am
content: The plane right below (around 200um typical) creates most of the capacitance you are fearing. The extra from the sides of the tracks is minuscule. The track coupling to the reference plane dominates the impedance.Also the shielding effect of added top fill is minuscule. If you can fit a shielding track between two tracks that would crosstalk, the distance itself offers almost the same effect without the ground track between. For example, with typical 6/6 mil rules, a track edge to track edge distance of 3*150um = 450um is required to fit a shielding track, but the ground plane is just 200um below and the surface area at 35um thick track sides is low compared to the surface area of the 150um wide track itself.Fill on outer layers requires proper ground stitching, otherwise you end up with floating antennas.When done properly (i.e., enough ground vias) it's OK to fill outer layers, but it's quite a lot of work for quite little gain; usually don't bother.

author: Miti
author_rank: Super Contributor
timestamp: March 27, 2021, 10:06:54 am
content: At work, we assemble boards for a big, known company, can’t say it’s name but is big. Their monster boards are all filled with copper, both outer layers.

author: Siwastaja
author_rank: Super Contributor
timestamp: March 27, 2021, 10:32:59 am
content: Outer layer having copper fill makes a lot of sense when it shields traces on the middle layer, creating a stripline instead of microstrip.But if mid-layer is also a ground plane, it doesn't make a lot of difference.In a power design, paralleling more copper on outer layers help reduce plane resistance, but this is only significant if you have room for such fill, but typically the top layer is occupied by all the components; and indeed, it tends to make more sense to utilize the top for placing components as tightly as possible, minimizing the distances and track lengths.

author: ebastler
author_rank: Super Contributor
timestamp: March 27, 2021, 06:48:18 pm
content: Thank you both! Sounds like the preliminary conclusion is: "Ground fill doesn't do much harm or much good" in this situation. I will probably put the fills, but with a generous gap to the traces.

author: miken
author_rank: Regular Contributor
timestamp: March 28, 2021, 12:06:09 am
content: Some older boards have copper squares, or crosshatched fills. I'm told that was to keep the etch more even, but with modern processes it's not necessary.Keeping the copper even on internal layers is important, though. Sounds like you've got that covered. I cut out an internal non-plane area on one of my first boards and it wouldn't lie flat

author: vad
author_rank: Frequent Contributor
timestamp: March 28, 2021, 03:42:40 pm
content: From manufacturing perspective it is always good to have copper fills on all planes.From signal integrity and EMI perspective, I would pay close attention to the signal plane that is close to power plane, if I were dealing with fast signal speeds / fast power transients measured in maximum dV/dt and dI/dt. And since you are concerned about trace capacitance, fast dV/dt is probably your case. Adding ground fill as close as possible to critical signal traces on the signal plane that is not coupled to ground plane would be my priority. Mitigation of trace capacitance should be achieved by means other than sacrificing good signal return path.

author: tszaboo
author_rank: Super Contributor
timestamp: March 28, 2021, 03:51:32 pm
content: Yes, if you have a lot of space on both sides, fill them up with copper, and connect it to GND. It is better for the board, as plating thickness will be more uniform. Mechanically it is better. Also more environmentally friendly, as that copper otherwise gets dissolved and uses more of the etching liquid. These are small differences, but they don't cost anything to do.There is one good reason not to fill boards: If you make a high risk prototype, where you expect drilling cutting or other changes necessary, in this case not having that extra copper helps.

author: radar_macgyver
author_rank: Frequent Contributor
timestamp: March 28, 2021, 04:03:22 pm
content: Another use for ground fills is to serve as a grounding point when using the blade-style low-inductance ground leads for active probes. Just scratch off the solder mask near where you need to probe.

author: Siwastaja
author_rank: Super Contributor
timestamp: March 28, 2021, 04:20:04 pm
content: You may want to use a larger-than-usual clerance for top fill, and/or set some neck/island removal rules, this way the fill doesn't get into every tiny gap, saving you from the tedious work of fitting gazillion stiching vias eating up space on all layers, or having long thin "ground" tracks flapping in the breeze.Filling just relatively large areas satisfies the etching uniformity recommendations and is less work.For example, if you normally use 6-mil clearance, 12-mil clearance for the top/bot fill saves you a lot of careful work.Still works as a prototyping grounding area with less risk of accidentally shorting tracks if you scrape off too much soldermask.