SparkFun Forums

[TokTok]

Hi all,

In my attached Eagle files i.e. schematic and board, I've got some unclear aspects feedback from my boardhouse in relation to my my ground plane and ground path.

1st issue: Firstly with the ground plane I'm being advised by my boardhouse that my ground planes and tracks are too close to the edge of the board. My boardhouse recommends 50 thou or mils margin. In all my previous board development attempts I've laid out my ground plane using the board outliune as my guide when laying it as you will notice from the attached board file or its screenshot.

Question: Does laying the copper pour with a certain margin away from the edge of te board affect the functioning of a board in any way?

Solution to the first issue: I'll lay the copper pour with a 50 mil margin away from the edge of the board.

2nd issue: My board house has identified the ground return paths for my Zigbee Module and PIC are all forced to follow a route around the bottom right corner of the board rather than a more direct path.

Question: Looking at the attached board file or screenshot what is the negative impact of having the ground return paths of my PIC and Zigbee module around the bottom right corner of the boardconverging

2nd issue continued: In addition they have mentioned if I were to concentrate on just one ground plane and try to keep all horizontal tracks on one layer even though this uses more vias I would have a less cluttered ground plane.

Question: Does this mean having a ground plane only on say the top layer not both layers?

Question: What would be the effect of having only one ground plane?

Question: How does having one ground plane make the ground plane less cluttered/crowded?

2nd issue continued: They also mention based on concentrating on one ground plane it would be more effective in its job e.g. L1 to COUT+ and L1 to F15 changing layer would give a more direct return path (use large vias).

Question: Why would having only one ground plane bring out better efficiency in the ground plane doing its job?

Here are the attachments:

SCH AND BRD.rar

SCH SCREENSHOT.png

BRD SCREENSHOT.png

Board screenshot.

I really appreciate any replies to the post.

[n1ist]

Running pours up to the edge lets them get damaged during routing. Running pours up to the edge of screw holes lets the screws short to the pours. That can be disastrous when you have a Vcc plane on one side and a GND plane on the other.

When laying out a board, you always need to visualize the return current flow in the ground planes. If it isn't right under the corresponding traces, you have more chances for EMI and noise problems.

You still haven't fixed most of the issues brought up in https://forum.sparkfun.com/viewtopic.php?f=20&t=38400

/mike

[Purple Squirrel]

1st issue: each board house is different in how they process/manufacture PCBs. That is why they have a set of manufacturing guidelines they will happily give you. However if you insist on them making your boards the way you laid them out they will most likely do so but tell you they are not going to warranty any of the work. So yes adjusting the copper pour with a 50mil space is the best way to go in this case.

2nd issue: ground return paths. the board house is trying to help you here. In regards to the PIC and Zigbee module they are presuming a rise time that is fast enough that your current layout will have trouble working with. The issue is the current loops that are created. You want to minimize them by keeping them as short as possible. Thus the more direct paths. If you had access to a signal integrity tool you could analyze your layout and make adjustments accordingly however most of us who use Eagle dont have that access.
As for the ground plane on one layer it has to do with how the signals on your board are referenced and this will affect how much noise you will see (this also refers back to issue 1).
For the record, use a single plane for ground.

Your question: Question: Does this mean having a ground plane only on say the top layer not both layers?
You do not want a ground plane on both layers. This will create a noisy and unstable design. It doesnt matter what layer your ground is for a two layer card.

Your question: Question: What would be the effect of having only one ground plane?
The result is a more quiet and function design.

Your question: Question: How does having one ground plane make the ground plane less cluttered/crowded?
What they board house was trying to say was less noisy. The ground plane is the return path for your signals. Current follows the path of least resistance (applies to slow rising signals) AND current follows the path of least inductance (applies to fast rising signals). in short if your ground plane is on one layer and has lots of vias the impedance is much lower than if you have your ground plane on different layers and with fewer vias.
Speaking of vias, you dont want them to be too big or to small for that matter. Vias have resistance, inductance, and capacitance and each of these values change with the size of the via.

your question: Question: Why would having only one ground plane bring out better efficiency in the ground plane doing its job?
refer to the above answers.


The thing that usually gets people when laying out a board is that they try to make the PCB layout look alot like the schematic. This is were alot of folks get into trouble. A schematic is nothing more than a picture of how things connect. The PCB layout is the physical result of that and is a component into itself. Change the PCB layout and you have changed the component.

There are lots of good resources for learning about PCB layout that you should look for. You may also find this website, http://www.sigcon.com, very useful.

Purple Squirrel

[davep238]

I've always used ground planes on both sides of the board, but I ALWAYS tie them together with vias. This gives better ground coverage. Check the datasheet for the wireless part. See the area with no pins? You aren't allowed to have any copper under that area of the part. Also, you should not have any top layer traces under the crystal except for traces that connect to the crystal. You do not want to have heavy currents flowing in the ground caps for the crystal, so don't have your heavy ground trace connected to them. Instead, use a separate ground trace connecting the caps to the micro-controller's ground pin, if at all possible. In other words, you want to have the crystal + caps isolated from the rest of the board. In a previous topic about this board, you had the micro-controller oriented differently, so that the crystal was away from most other traces. Give that a try. At the end of that topic, I uploaded a version with ground planes on both sides, but left the crystal alone (to save time). Take a look.