"window screen" ground planes? - Page 1
Forum section: electronics / general

author: NiHaoMike
author_rank: Super Contributor
timestamp: May 16, 2012, 01:56:28 am
content: I have an old PCB (a DSerial PCI card to be exact) where the ground plane looks like a window screen. Is that just to give it an "interesting" look? I remember that last time I tried to use it (many years ago), it would only work properly in some computers, generally disliking ones that had many PCI devices. Might that have something to do with the increased ground plane impedance? Interestingly enough, there is a solid patch of copper under the crystal.

author: Psi
author_rank: Super Contributor
timestamp: May 16, 2012, 02:00:20 am
content: I believe hatched ground planes were just because some pcb design software didn't support solid pours. So they did a crisscross of tracks instead.

author: AtomicDog
author_rank: Newbie
timestamp: May 16, 2012, 07:06:30 am
content: RF will see a screen as a solid surface. A Faraday cage is an example of this.

author: free_electron
author_rank: Super Contributor
timestamp: May 16, 2012, 10:11:21 am
content: The reason for those is not what you might think... It originates in pcb manufacturing technology.Making a good reliable attachment between copper and the isolation material can be difficult. Especially if you process control is bad...On multilayers this is a common problem. The copper needs to be roughened up to let the next layer 'stick to it' or the layers would peel off.When soldering the board in reflow you can get a kind of popcorn effect: the layers separate and the board balloons...Large solid slabs of copper give trouble... So they solved it by shooting holes in it. That way the next layer of isolation material can bond with the isolation material underneath the copper and make a better mechanical bond.The added bonus is that there now is also less thermal mass to wick away heat during soldering. The temperature cycle can be shorter , soldering is faster and there is less chance of the board popcorning.For emc or signal integrity it doesnt really matter. It is still a faraday cage.

author: EEVblog
author_rank: Unknown
timestamp: May 16, 2012, 11:45:32 am
content: Quote from: Psi on May 16, 2012, 02:00:20 amYes, that is one of the reasons, and some manufacturing issues too as Free Electron pointed out.Some designers also just prefer the look of it, so you still see it occasionally today even though the manufacturing issues don't really exist any more.Dave.

author: ejeffrey
author_rank: Super Contributor
timestamp: May 16, 2012, 12:22:56 pm
content: At least it doesn't matter for most digital circuits. For analog microwave circuits you definitely want a solid pour. At that point you aren't using FR4 either.

author: free_electron
author_rank: Super Contributor
timestamp: May 16, 2012, 12:56:12 pm
content: Quote from: ejeffrey on May 16, 2012, 12:22:56 pmAnd why not ? There are plenty of fr4 materials suitable for microwave work.FR4 is just a classification... This is one of the largest misunderstandings in things pcb related.Fr means fire retardant category 4.There are hundreds of different fr4 materials. Each can have different resins and a different weave of the material. It is the weave that has the largest impact when it comes to rf. the density of the material changes depending on where the strands are. So you get discontinuities in the impedance. If you select a tight weave with fine strands and you stack thin sheets under 45 degree angles you can get a really uniform buildup that works perfectly fine deep into the gigahertz range.The worst you can do is route the traces in line with the weave. Take a differential pair for example. One line runs on top of a thick end , the other on top of a valley . There will be noticable differences in flight time. And you will get signal skew. Your differential signal is no longer differential !The solution is to make a prepreg stack made from thin sheets with multiple angle rotation , or route the traces in zig-zag so that you cross strands and valleys ( rule of thumb is that the zigzag amplitude needs to be 3 times the strand width.Even materials such as isola, rogers Nelco or getek employ fiberglass cores but they are scattered or randomized to eliminate the problem. Actually Getek is also classified as FR4 and is one of the most used rf substrates out there. The same goes for Rogers 4000 and other series. They are also classified as FR4. FR4 is just a classification for flammability. Nothing else.Typically a board with a dense weave like 2116 will perform better than let's say a 106.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: May 16, 2012, 01:01:20 pm
content: My understanding is that non-solid planes were common in the days when through-hole dominated, as the wave-soldering process caused bubbling, but nowadays with reflow it's not an issue - presumably due to the much slower heat-up and cool-down rates. Possibly also improvements in PCB materials to cope with SMT processes.Another very minor consideration is that it costs slightly more to etch off more copper, so solid is fractionally cheaper, but only when dealing with high volumes.

author: free_electron
author_rank: Super Contributor
timestamp: May 16, 2012, 02:04:07 pm
content: Quote from: mikeselectricstuff on May 16, 2012, 01:01:20 pmactually solid is more expensive ... mass pcb producers use ammoniumpersulfate to etch. this is a regenerative process and they can extract the copper back out of the etchant... that copper can then be used in electroplating for example.like you said : non solid planes are better for wave soldering . no need to muck around with thermal reliefs. but is it aslo true for SMT.

author: NiHaoMike
author_rank: Super Contributor
timestamp: May 17, 2012, 05:18:59 am
content: The date codes on the chips suggest that board was made in late 2000 or early 2001. It's only double sided (typical of simple expansion cards back in the days) so there are ground planes on both sides of the board, with lots of cutouts for various traces. Cutouts in ground planes can easily cause signal integrity problems at high speed, especially on a ground plane with a high impedance, so I added jumpers to bridge across cutouts in the ground planes. I also added some more bypass capacitance. The fact that it does not seem to like busy buses (IIRC) makes me think it's a signal integrity issue.