I am making a shield for the Maple, and it has some high voltage (relatively, 12V) and low voltage signal/power traces. I am wondering if I should have a ground plane. I have a two-layer board, and I am only using the reverse side. ExpressPCB insulates all traces and pads automatically when I add a ground plane, so could I put it on the reverse side also and possibly reduce cross-talk between traces? Thanks.
Cross-Talk and Ground Planes
(26 posts) (5 voices)-
poslathian
LeafLabsThis is probably a good idea. It depends on how high bandwidth signals you expect on the topside traces. Even signals in the KHz will start to bleed. On Maple Rev1, when we only had 2 layers, and generally a layout that couldnt afford to have large and isolated power and ground planes we had a lot of crosstalk. Many fast digital boards, such as this DLP FPGA board on my desk (which is probably 6 layers but still poorly designed) have terrible crosstalk between traces that have lots of overlap or run too closely together...to the tune of 80mV!
Posted 5 years ago # -
Silntknight
ModeratorOk, I'll throw in a backside ground plane. I actually have no traces on the topside. I was considering making that a power plane, but I'm not sure how that would affect some of my devices, like capacitors and DIPs. Maybe I could just exclude those sections. Or, I could put all the traces on the topside along with the ground "plane" (I guess it isn't a true plane if it is a two layer board) and put a power plane on the backside.
Posted 5 years ago # -
gbulmer
Moderatorposlathian -
Even signals in the KHz will start to bleed.
Interesting you write that here. When i was suggesting the RTC crystal signals stay on the PCB and be tracked, partly because of noise, you suggested it was not a problem
Am I misunderstanding? Have you since measured the PCB, and found it is a problem? Or is this something else?Silntknight - what is it you are trying to achieve?
What sort of signals are on the shield, and how dense is it?If the signals are a mix of analogue and digital, high-current vs low-current, high-frequency vs low-noise, there is more to it than "putting on a ground plane".
A ground plane will allow you to reduce electrical noise (with proper routing), and make it easier to route ground.
If you can route the board with nice thick power traces on the signal side, then I don't think a power plane will have as big effect an effect as a ground plane.
If the board is all through hole (you say "I actually have no traces on the topside"), then put the ground plane on top.
AFAIK, component placement has a much bigger impact than any other issue.
But hey! I'm not an EE ;-)
Posted 5 years ago # -
in general, a ground plane is always a good idea when possible.
it makes routing to ground easy, and you and you can use vias to gnd to provide noise isolation for traces.
a power plane, while it makes routing easy, doesn't provide the same isolation benefits, and could actually just form a giant capacitor with the ground plane, so unless you're doing 4 or 6 layer, it's probably not a good idea.
if you have room on top and bottom, put the ground plane on both layers, and use thick traces for power.
Posted 5 years ago # -
Silntknight
ModeratorGbulmer, the shield is pretty dense, IMO. The traces are actually very large for the current they run. They are each 1.02mm traces. There are a 4 PWM outputs, 3 analog inputs, and 2 digital inputs. They are all low current; I moved higher current stuff off the shield and onto breakout boards.
Soundcyst, if the backside is fairly dense, should I still put a ground plane there? I think that placing one should reduce cross-talk.
I am also putting a link to a picture of my board. Keep in mind that this was my first attempt.
The large 16-pin DIP is an optoisolator. The two 8-pin DIPs are MOSFET gate drivers. The only TO-220 in here is a 5V regulator. Also, this is without the ground plane on the front side (as it would block everything) or on the backside.
http://i1221.photobucket.com/albums/dd470/Hari_Ganti/Supermileage%202010/EMU.jpgPosted 5 years ago # -
Silntknight
ModeratorFYI, I realized that my Hall sensor needed some decoupling, so I am actually going to move all the decoupling and resistors (for the analog sensors) off board to smaller breakouts. Only the signal will travel to the Maple. Maybe I'll save some room. In that case, I might connect the 5V regulator directly to the sensors and have the raw battery power go in the barrel, which I saw suggested elsewhere. This kinda sucks because I already ordered my parts and I can't cancel my order, even though it hasn't shipped. I don't want to pay shipping twice!
Posted 5 years ago # -
poslathian
LeafLabsgbulmer - the bleed I was referring to was just what Ive seen on lots of dev boards, including Maple rev1. Were quite pleased with the noise performance on rev3 and later, which was mostly gained by upping to 4 layers, isolating digital and analog power planes, and generally being more careful. On a two layer board theres just less room to add backplanes or generally be careful with the routing.
Running the RTC out to external...well...first off its a digital signal, so its not the end of the world if youre getting 50mv of crosstalk, which is the point of digital - the old static discipline and all. Also, okie did a nice job of giving those pins plenty of room in their own little corner to break out, which puts most of the noise burned on what happens when those signals leave the board - namely the design of the shield. Eitherway, becuase RTC clocks are slow and the signal is digital it really shouldnt be a problem.
What is a problem is when you have a 10 bit ADC pin, sitting next to a digital pin which is injecting 60mv of crosstalk onto the analog pin - effectively deleting half of your analog resolution! We are VERY pleased to be getting all 10 bits out of most of the ADC pins, I dont think it would have been possible on a 2 layer board unless there were many var fewer pins and components (for example the maple mini) EDIT: [actually maple mini is 4 layers...]
Posted 5 years ago # -
gbulmer
ModeratorSilntknight - without the schematic, I find it difficult to be definite.
When I wrote "component placement has a much bigger impact than routing", it was serious. If the basic component layout avoids noise, then the battle is almost won.
That board looks like all of the analogue tracks (the ones that will pick up noise) are routed from lower right to left, then almost top left. They wrap around the PWM and digital signals (which will be one of the sources generating noise).
I'd be tempted to do a few things:
1. Plan to make several prototypes, to test things, and budget for rework.
2. Move the parts around.
Move the analogue subsytem components close to the analogue pins, (i.e. to lower right), and move the digital subsystem components towards top left. Maybe move some of the digital/PWM I/O from the top right header to the top left header too. Bring digital and analogue signals out on opposite sides of the board, where feasible. It looks like the two subsystems can be completely segregated.Then worry about ground planes. If the subsystems are very cleanly separated, and it looks like there is enough space to do it, the board could have an analogue ground plane and digital ground plane which will not intermingle.
What is the minimum clearance and track width that the PCB manufacturing process can reliably handle? (just wondering what else will fit). Maybe put some test points in, so it is easy to attach oscilloscope probes.
My $0.02 - HTH
Posted 5 years ago # -
Soundcyst, if the backside is fairly dense, should I still put a ground plane there? I think that placing one should reduce cross-talk.
it depends. it's worth a try to see how much of a plane you'll actually get. you may need to add vias to avoid orphans, and you may need to change the size of your traces to fit a via between them, but in general, it's better to have ground in between your signals.
gbulmer's dead on about oscilloscope test points, and expecting to make several prototypes. very rarely do engineering endeavors like these succeed on the first time. ("like these" meaning designing shields, not your particular application)
if you're trying to save $$$, it might be worth getting an adafruit protoshield and doing some point-to-point wiring to make sure your circuit will do what you think it will.
Posted 5 years ago # -
Silntknight
ModeratorThanks for the advice. Because of some new information I received (namely the Hall Sensor business), I am actually going to rework most of this. I'll try to keep in mind the changes you all suggested. Also, making a ground plane will make this a LOT easier. The ground traces gave me a lot of trouble earlier. Also, I plan to make the board myself. I haven't found a company that will let me build a single board for a few bucks. That also means vias are a little more difficult. They'd just be holes filled with solder.
Gbulmer, I understand that placement is essential. That is why I asked about all of this. Sorry to inform you, but the schematic is actually incomplete because I added a ton of components after I initially drew it. I used this program because I thought it was capable of auto-routing, but I couldn't find the feature. I just routed it myself.
Posted 5 years ago # -
Silntknight
ModeratorIt took a few hours, but I redid it. Check the images.
http://i1221.photobucket.com/albums/dd470/Hari_Ganti/Supermileage%202010/BreakoutBoardsBottomLayer.jpg
http://i1221.photobucket.com/albums/dd470/Hari_Ganti/Supermileage%202010/BreakoutBoardsTopLayer.jpg
http://i1221.photobucket.com/albums/dd470/Hari_Ganti/Supermileage%202010/ECUShieldBottomLayer.jpg
http://i1221.photobucket.com/albums/dd470/Hari_Ganti/Supermileage%202010/ECUShieldTopLayer.jpgNote to the Leaf Labs Team, on-site image hosting for posts might be useful.
Posted 5 years ago # -
gbulmer
ModeratorI plan to make the board myself.
Depending on the facilities you have access to, it may be much easier to make a single sided board.
I haven't found a company that will let me build a single board for a few bucks.
AFAIK, Sparkfun's batchpcb is one of the cheapest ways to make one off boards.
http://batchpcb.com/index.php/FaqI've never used it, but a friend has, and said it was pretty good.
That also means vias are a little more difficult. They'd just be holes filled with solder.
Doing it with solder alone will be difficult.
We use the offcut leads from thru-hole components, e.g. resistors.I used this program because I thought it was capable of auto-routing, but I couldn't find the feature.
Eagle autoroutes, but for any useful level of complexity (e.g. for microcontroller board), it is almost useless. I find it is helpful to see it autoroute a couple of signals at a time, then rip them up and do them by hand.
I work with folks who use Protel. They route power and ground, and critical signals, by hand then let it autoroute the rest.Posted 5 years ago # -
mbolivar
LeafLabsNote to the Leaf Labs Team, on-site image hosting for posts might be useful.
Thank you for the suggestion. Right now, however, we're trying to keep the number of services we host directly down to a minimum, so as to devote the maximum number of hours possible towards libmaple, maple-bootloader, etc. We plan on revisiting the question of what to host ourselves as the platform starts to mature, so comments on what's desired are welcome.
Posted 5 years ago # -
if you're in the US, visit http://pcb.laen.org
laen's prices are cheaper than batchpcb's for 2-layer boards under 4 square inches (2x2). for 4-layer boards, laen is cheaper for anything 5 sq inches and under.
the biggest difference is, you get 3 copies of your board, so if multiple copies are necessary, it's actually 3x cheaper than batchpcb.
he also includes shipping at that price, and the boards are made in the USA, instead of in china, which is nice for our economy and such..
Posted 5 years ago #
Reply »
You must log in to post.