buried bias and power planes v/s old fashion IC power  - Page 1
Forum section: electronics / general

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 03:06:30 am
content: I just send a budget for a PCB that have tons of buried bias (never done it before) and are WAY more expensive than a regular PCB, and with regular I mean draw tracks to power chips and stuffs, and not getting the power from power planes.I did it because the specifications for RF chip recommend some 4 layer PCB as best, and impedance matching for RF tracks for certification later (CC3200MOD).There is a way to manage the buried bias and not get plucked on the process ?, o a better alternative not so expensive ?I have no experience on this, so any tip is welcome.Thanks.

author: JJalling
author_rank: Unknown
timestamp: March 15, 2016, 10:38:24 am
content: Can't you just make the vias go all the way through the PCB, instead of burying them? Or am I misunderstanding the question?BR Jonas

author: dmills
author_rank: Super Contributor
timestamp: March 15, 2016, 10:44:01 am
content: Edge rates these days mean that my default starting position is 4 layers (Two layers is only for almost literally DC power and smallish audio things and even then....).Buried via is insanely expensive, sometimes you have to, but on anything you can reasonably route in 4 layers you should be able to avoid it.4 Layer is pretty much the minimum for acceptable performance if the board is even slightly non trivial, and should not add that much to the cost if you are doing a reasonable sized run (There is rather more setup involved).If you want sane prices at small volumes then you must make sure the options you select match the board house defaults for a 4 layer, but for RF you will want to use someone who specifies the layer stackup so that you can calculate the track widths for the appropriate impedances.I can and have done two layer RF boards (One routing layer plus ground plane on the back, the trouble is if you do this with a 1.6mm FR4 board, a 50 ohm trace becomes insanely huge, and even a 1mm or 0.8mm thick board does not really solve this, a buried ground plane say 0.2mm under the outside routing layer however, and all of a sudden your RF tracking is a sane size.The ground plane is kind of non optional IMHO so a two layer stackup only has a single routing layer, where a 4 layer has two (And you can sometimes sneak some routing onto the power plane remembering that signals on the back of the board will be using the power plane as a reference so chopping it up is not a great plan, so effectively two and a bit).Regards, Dan.

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 02:28:53 pm
content: Quote from: JJalling on March 15, 2016, 10:38:24 amYes I can, but the real problem is my projects become more and more complex and I have to deal with this problem, plus I expend too much time arranging tracks. And as far I know, vias (TH) are not the best solution to get contact to mid planes.

author: tszaboo
author_rank: Super Contributor
timestamp: March 15, 2016, 03:59:05 pm
content: You should first think about going 6-8 layers or HDI before buried and blind vias. If you have to use a 4 layer stackup for some magic RF reason, than I would rather use a 8 layer board and skip layer 2, making it 7 layer board, with similar stackup:TOP RFNothingGNDLayer4Layer5Layer6Layer7Bottom4-5-6-7 is up to you. Maybe even sacrifice the third layer. Buried and blind via only when PCB size is defined by the marketing department (giant phones, anyone?). This will probably change in a decade or so.

author: wraper
author_rank: Unknown
timestamp: March 15, 2016, 04:17:16 pm
content: Quote from: Morgoroth on March 15, 2016, 02:28:53 pmIt's the normal way for the most of the boards. Buried vias are for cases that design is so dense that there is no space for normal vias. And why the hell you need buried vias on the 4 layer board at all? Even blind vias is something extreme with only 4 layers. I would understand if there was 8+ layers, board full of BGA and no space for normal vias, but 4???

author: T3sl4co1l
author_rank: Super Contributor
timestamp: March 15, 2016, 05:13:48 pm
content: Controlled impedance does nor require buried vias, nor does it require any of the goofy stackups people are suggesting in this thread...The only reason it's not typically feasible on 2 layers is because the trace width is unusually large (30-60 mil for 50 ohm). There is no problem with EMC on a properly poured and stitched 2 layer board.Tim

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 05:44:46 pm
content: Quote from: wraper on March 15, 2016, 04:17:16 pmbecause the app notes of CC3200MOD recommend use 4 layers for many reasons,not only RF, and 4 layers mean blind vias at least. Other option is to use TH vias to reach power layers on middle of the stack, but as I know that is not recommended. If I'm wrong please let me know.I just did put vias on without any consideration because I wasn't aware of the price related to them (very noob trap?). Now I've deleted and replaced all buried vias for blind bias without problems.

author: Kilrah
author_rank: Unknown
timestamp: March 15, 2016, 05:50:56 pm
content: Quote from: Morgoroth on March 15, 2016, 05:44:46 pmWhy? Every board I have in front of me here uses TH vias to access the middle layers, none of them needs anything more advanced, even with big fat BGAs.No reason to use blind vias unless you're doing something so tight that you can't accomodate the "waste" of space they cause on all layers, or have extremely fine pitch BGAs.

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 05:56:20 pm
content: Quote from: T3sl4co1l on March 15, 2016, 05:13:48 pmYou'r right, huge trace width at 2 layer stack.

author: langwadt
author_rank: Super Contributor
timestamp: March 15, 2016, 05:56:32 pm
content: Quote from: Morgoroth on March 15, 2016, 05:44:46 pmTH vias are the standard, unless you a building very high density PCBs or using super fine pitch BGAs, there is not much reason to use blind and buried vias

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 06:12:03 pm
content: Quote from: Kilrah on March 15, 2016, 05:50:56 pmI'm asking just because I don't know and I don't have other place/people to ask, in this country nobody close to me has experience on develop and manufacturing electronics.And I've read so many documentation that I can't tell you precisely where I get the idea of not to use TH vias to get middle planes, plus there is a bunch of people giving advice not so accurate sometimes, for sure with their best intentions, and I must be a bit cautious, and that is another reason why I'm here.So if is OK to use TH vias, I'll fix my PCB on that direction then.Thanks.

author: wraper
author_rank: Unknown
timestamp: March 15, 2016, 06:44:24 pm
content: Quote from: Morgoroth on March 15, 2016, 05:44:46 pmLOL what? That datasheet even mentions how to use it on the 2- layer board. Why 4- layer board = blind vias is just beyond me.

author: m98
author_rank: Frequent Contributor
timestamp: March 15, 2016, 10:59:32 pm
content: Quote from: Morgoroth on March 15, 2016, 03:06:30 amHow did you come to the conclusion that you'd need something like buried vias for such a simple application? I just don't get it. The suggested transmission line design from the datasheet just shows regular ground stitching going through the whole PCB.

author: Morgoroth
author_rank: Regular Contributor
timestamp: March 15, 2016, 11:13:16 pm
content: I think I read too much garbage and got confused, indeed I re read the docs and you'r right.

author: exmadscientist
author_rank: Frequent Contributor
timestamp: March 16, 2016, 02:27:11 am
content: For what it's worth, I've gotten the CC3100 (extremely close to your CC3200) working just fine on 4-layer prototype boards from OSH Park, no buried or blind vias anywhere to be found. It worked just fine, with plenty of signal strength.