Any downside to double sided ground plane? - Page 1
Forum section: electronics / general

author: Circlotron
author_rank: Super Contributor
timestamp: May 10, 2016, 02:25:50 am
content: Whenever I draw up even a relatively simple board I always pour a ground plane on both sides. This makes things easy from the point of view that I don't have to be overly concerned about how to get a ground track to everywhere it has to go. Also makes for great low impedance earth run. I am very aware of the significance of ground loops and coupling through shared earth runs. Thirdly, it doesn't consume so much etchant because only relatively little copper has to be removed. Why waste it for no good reason, even if someone else is doing the board manufacture?Anyway, is there a downside to having a ground plane if it is not absolutely necessary? Any stuff with a decent bit of voltage I raise above the board, and am aware of the extra heat needed to solder & unsolder some connections.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 10, 2016, 04:49:19 am
content: Nope*!*Consider what you are doing. If the planes are well stitched, and surround all traces pretty well, then all the traces are nice transmission lines, specifically coplanar waveguide construction. At typical dimensions, this lands in the 70-100 ohm range, which is quite reasonable for most CMOS digital stuff.You also get isolation between traces, at least if there's enough clearance between traces that ground pours inbetween them (for at least a trace width, and via-stitched in at least two places). If not (running traces together in bunches on the same side), isolation isn't good but it's still more than fine for CMOS signals.And as such, if your circuit has an impedance very different from the transmission line impedance, then every bit of trace length will matter. A very high impedance circuit, like an oscilloscope front end, or a very low impedance circuit, like a high current switching power supply, will need much wider conductors and careful limits on trace length.So a high impedance circuit might need greater clearance to (top) pour, thinner traces, and even no (bottom side) ground plane at all, for best results. The downside is more crosstalk, so you need to work accordingly.Tim

author: Richard Head
author_rank: Frequent Contributor
timestamp: May 10, 2016, 06:25:53 am
content: I would go so far as to say it's beneficial. Removing large amounts of copper on one side of the board and not the other almost always results in bowing of the board. The pick and place machine then has to try to place components on a banana. There is a section in the IPC standard that deals with this issue.

author: coppice
author_rank: Super Contributor
timestamp: May 10, 2016, 06:39:11 am
content: Leaving copper behind doesn't waste etchant. Commercially the etchant is reconstituted, and the copper recycled. So, removing more copper actually cuts costs. However....From the electronics point of view its usually better to leave copper in place as extra ground plane, so long as all the pieces are properly connected together. Isolated bits of copper foil are more like antennae than ground plane. Not all ground planes are created equal. You need to know what you are doing to make them really effective.

author: Richard Head
author_rank: Frequent Contributor
timestamp: May 10, 2016, 07:21:37 am
content: Isolated bits of copper foil are more like antennae than ground plane.That is true unless you select "Remove unconnected copper" in CAD.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: May 10, 2016, 05:43:56 pm
content: Form a manufacturing angle, you ideally want a similar amount of copper on each side. On thin boards in particular, an unbalance can cause warping during reflow.

author: linux-works
author_rank: Super Contributor
timestamp: May 10, 2016, 06:56:22 pm
content: glad I read this thread; I didn't think that board bowing would happen. good point! I don't do pcb for a living, so this is a new tip for me. thx