Favour more vias or longer traces on other side? - Page 1
Forum section: electronics / general

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 08, 2016, 08:12:37 am
content: I am laying out my first two-sided board (after years) for a small 20MHz Z80 computer. I have most of the buses routed and am trying to connect the last nets. I find myself confronted with the choice to have more via's in order to keep the ground plane on the other side as big as possible or to have somewhat longer traces through the ground plane.I expect there is no golden rule, but is there a best practice or some rule of thumb when to favor the one over the other?If it matters: Im using KiCad 4 on standard settings...

author: matseng
author_rank: Frequent Contributor
timestamp: March 08, 2016, 10:27:17 am
content: Looking at Z80-era boards there seems to be no ground planes at all unless the pcb is large and sparsly populated. It looks like they usually first route the vcc/gnd between the IC's (which are put in nice long straight rows). And then just route the rest of the board as needed with what looks like 12 mil tracks. With decoupling caps at each IC it worked just fine back then. With the same class of parts/speed I see no reason why it wouldn't be find today as well.

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 08, 2016, 10:36:26 am
content: Well, the clock speed is a bit higher nowadays and I gathered from others on this forum that a ground plane is "always" a good idea.The question was more intended to be more general than my specific project. My project just triggered me into asking the question...

author: tszaboo
author_rank: Super Contributor
timestamp: March 08, 2016, 10:47:25 am
content: You can use single layer with jumpers, obscure color silkscreen, TH capacitors, FR1 board, and probably the thing will still work.

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 08, 2016, 12:24:24 pm
content: Thank you, you totally did not answer the question.

author: AndersJ
author_rank: Frequent Contributor
timestamp: March 08, 2016, 01:00:48 pm
content: For "long" rise and fall times, and low current signals I would use a longer tracerather than compromising the ground plane.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 08, 2016, 02:41:32 pm
content: Vias are cheap (zero cost in prototypes, anyway).You don't need solid ground plane, but it should fill around all traces without too much open area of just traces (or footprints) on both sides. Via stitching spans the gaps.If you have a low density board, it's reasonable to confine all traces to one side, except for a few 'jumpers' that pass to the opposite side. All remaining area (the negative space around the traces) fills with ground. As density increases, more and more traces have to follow crossing paths on both layers, and you will have more intersections where ground is excluded. As long as these areas aren't too big, your signal quality is still good.I would much rather have good signal quality in the PCB, even if it isn't a priority for the technology used (~ns edges from HC or LS logic over < 40cm trace lengths). Pretty much everything historical had to be enclosed in a metal shield to meet regulations. Which is really just a crappy way of implementing more ground planes!Tim

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 08, 2016, 03:22:36 pm
content: So you have a ground plane on both sides? Oh, I was planning on making the back side ground and the top vcc...? Not a good idea?Ok, via's are cheap and are preferred over breaking up the ground plane too much - that is what I read from the responses...

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 08, 2016, 05:34:10 pm
content: Here some screen shots to get an idea of my layout.The spare room on the right is reserved for more stuff.

author: jolshefsky
author_rank: Regular Contributor
timestamp: March 08, 2016, 06:23:38 pm
content: I have wondered about this myself. I "discovered" the model of using one direction traces on one side and perpendicular traces on the other (e.g. front is up-down; back is left-right). One side would have a ground plane and the other a power supply rail since any low-impedance power source is AC coupled to ground. The orthogonal traces tend to let the plane flood everywhere without hassle.I know enough to know that this isn't going to fly with very high frequency stuff; should I need to do anything above a few dozen MHz, I'll need to learn more or have someone else do it for me.One comment: it looks like your traces are all very skinny, perhaps 8 mils. That may be the minimum for your fab, but maybe go with 10 mils or 15 mils to avoid any problems (maybe a corner gets etched away by accident, etc.) (Side note: since KiCAD's DRC tends to complain for what is essentially rounding errors, I set my trace widths to 9.9mils, 19.9 mils, 39.9 mils, and 99.9 mils although I usually route with 19.9 mils for signals and 39.9 mils for power unless I have reason to do otherwise.)

author: obiwanjacobi
author_rank: Super Contributor
timestamp: March 09, 2016, 08:57:04 am
content: I just used the default KiCad settings for traces. I have to route between pins and in the zoomed in screen shot you can see I almost hit the margin of the pins. I will make the traces bigger when I am fairly certain it will fly. Thanx!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 09, 2016, 01:45:00 pm
content: You really ought to have one complete layer of unbroken supply (usually ground for obvious reasons), which means at the very least, a whole lot of stitching (with vias and traces) to repair the holes in a single layer. At which point you'll have so much on the opposite side that you might as well pour it, too.You'll have to do both to use a supply on each side. Plus all the traces going around them, which will be very confusing to design (if not impossible). It will certainly take up more area.On 2-layer construction, I prefer to route VCC as just another signal trace, with a suitable width (since it's carrying more current, after all). The bypass caps (which don't really even need to be one-per-chip for this technology) serve to anchor those traces to the ground plane, which with pouring on both sides plus stitching, is now almost as solid as a 4-layer board's ground.Using about N/2 layers for supplies and N/2 for signals seems to be pretty reasonable. Within a taller stackup, you can shift order and purpose to suit (six layer with [signal 1, GND, signal 2, signal 3, VCC, signal 4] is very common), minding that you get a little crosstalk between traces that are allowed to overlap (whereas an every-other-layer-VCC/GND build has full shielding between all layers).A two-layer board is kind of a special case, because you need at least two layers to comfortably route traces (i.e., without resorting to jumpers like a loser). But that leaves you with <1 layer to reserve for only one supply. Which is to say, no matter how you pour it, your ground is likely to have holes. So you might as well make the best of it and pour everything you can, and stitch it so it becomes one contiguous layer again.Tim

author: KL27x
author_rank: Super Contributor
timestamp: March 15, 2016, 05:55:05 am
content: If you run longer tracks through the ground plane and run into any problems, you can always stitch up the ground plane on a one-off with a sharp knife and some 0R 0805 resistors.Which way would I do it? First I'd check with my PCB manufacturer to see if number of holes is part of their pricing formula. If not, I'd go with more vias.

author: obiwanjacobi
author_rank: Super Contributor
timestamp: April 18, 2016, 09:31:47 am
content: O0