Question about Stackup and high voltage - Page 1
Forum section: electronics / beginners

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 16, 2020, 05:08:08 am
content: I'm conceptually trying to determine a proper stackup for a PCB project involving high voltage (less than 1 kV), and I found this stackup below on Stack Exchange.https://electronics.stackexchange.com/questions/137580/high-voltage-pcb-designLooking at the markup, the poster has signals and power on the top two layers, ground in the middle, and high voltage traces on the bottom. This may be too simplistic of a question, but when you devote two layers to specific signals, like how the mock up shows, what do you do for the ground pour? Do you tie it to ground, or do you not tie it to any net? Wouldn't leaving it untied create unwanted copper islands? That's something I never understood. People say that for four-layer boards, you should separate your signals, but I never understood what do for copper pours, aside from tying them to ground on all layers to reduce the impedance.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 16, 2020, 11:44:12 am
content: Stackup doesn't matter, the thru-plane insulation is more than enough -- but, you will want to use a custom stackup as proto stackups are a bit too thin for comfort at those voltages.A classic example, I have a deflection board pulled from a Trinitron monitor -- there's a few traces with up to 1.5kV DC or peak on them (some for focus, some carrying the powerful deflection signals). The board is 2 layers. What they've done is slather silkscreen over the critical traces, give generous creepage distance to surrounding ground/signals (and yes, ground is ground, don't leave floating metal), and slots are routed through the board where traces or pins can't be kept far enough away to meet creepage.The traces definitely carry real voltage: there's a subtle film of dust, electrostatically bonded to those traces.So that leaves creepage and clearance, and yeah, there are rules for that, depending on application, coating, etc.For example, UL/IEC 60950-1 requires that a coating be inspected, otherwise bare creepage rules apply. The coating might be soldermask, silkscreen, conformal coating, etc. Whereas any bulk-fill insulation is typed a "cemented joint" -- this includes internal PCB traces and potting.True story: at a PPoE, a predecessor had built a few prototypes with ExpressPCB. Including an industrial switching module, putting 650VDC across planes of a 4-layer proto board. He used default 7 mil clearance on inner layers! One or two of the boards failed shorted, the other handful worked just fine (at least for what little time they were operating).I certainly can't recommend spacing or layer thickness this low, but it goes to show you, the materials can perform quite well. The problem is defects causing early breakdown. The cure is following recommended separation, more like 30 mils internal, 100 mils or more external. Then you have something that can be produced, in quantity, with confidence.Tim

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 16, 2020, 03:36:28 pm
content: Thank you for your reply. If you don't mind, I'm confused about some terms.First off, what do you mean by proto-stackup? My go-to is the stackup from OSHpark 4-layer service, but I know that Advanced Circuits has varying stack-ups for multi-layered PCBs, with the difference being the overall thickness and varying core based on the number of layers.https://www.4pcb.com/pcb-stack-ups-.125.htmlSecond, from what I can tell, a slot is more-or-less a plated through-hole. Would simply using a plated-through-hole in place of a via be more than enough to traverse layers for high-voltages?Lastly, regarding your story about the prototypes, is that clearance between traces on the same plane and/or traces to the ground pour? Increasing the clearance for traces seems easy enough to do with no-fill zones, if it's only for high-voltage traces.So, from what you said, with high voltages, best practice is to ensure that high voltage traces are separated sufficiently from other non-high-voltage traces (creepage). Otherwise, it's fine to make all copper pours ground (no floating metal). Is this an adequate summary?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 16, 2020, 04:16:54 pm
content: Most places have a proto stackup that's something like, 1.6mm total thickness, 0.5oz inner, 1oz outer, with 0.18mm prepreg between core and outer layers. So,top soldermasktop 1oz copper0.18mm prepreg0.5oz copper1.2mm core0.5oz copper0.18mm prepregbottom 1oz copperbottom soldermaskThe prepreg layers are rather thin for high voltages between mid and outer.You can order different stackups just fine, but mind you have to order themfull customand they will be more expensive. That's how I ordered this board from PCBCART, around $200 for ten.https://www.seventransistorlabs.com/Images/ResonantGateDriver.jpgYou could also order as a 6-layer board with nothing on the mid-surface layers, but these are usually made with prepreg in the middle so the middle plane layers may not have much voltage rating (usually, the two middle layers are intended for extra signal routing, and the mid-surface layers are the planes). YMMV.Tim

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 17, 2020, 03:32:24 am
content: Dang. That's a lot to consider. Seeing as how I only need only just a few boards, I was hoping that I could not have to go a custom PCB route.Thank you again for your replies and responses. I'll take your advice and experience into consideration as I layout my board. With any luck, I can add some things, remove some things, and just simply make it easier for working with high voltages. Luckily (or at least, I'm assuming) my high voltage traces won't draw a lot of current (probably no more than a milli-amp or less), so all I can focus on is clearance and creepage. Thanks again.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 18, 2020, 04:49:23 pm
content: Sorry for the message again, but I wanted to ask another question regarding pin clearance with high voltages.I was playing around with Saturn's toolkit. Looking at the conductor spacing, assuming Device B2 at 301-500 V, the minimum conductor spacing is calculated to be 0.25 mm. Now, applying that to a 2x7 header, there are some headers with a pitch of 2.54 mm as shown below. However, applying that to female jumpers so that I can jump two pins together, with a pitch of 2.54 mm, I'm limited to a max of 300 VAC for the voltage rating. The header and jumper are going to act as a high-voltage selector of sorts, like a MUX, where the jumper selects one voltage to output out of seven inputs, so if the jumper is 'in series' with the high voltage, the voltage rating doesn't matter for the jumper, correct?https://www.digikey.com/en/products/detail/omron-electronics-inc-emc-div/XG8W-1441/1829468

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 18, 2020, 08:35:13 pm
content: I wouldn't recommend high voltages on fine headers. You could skip every other pin, which is fine for connectors; but useless for jumpering. Or you can get a bigger one (0.156" or 0.2"), or an industrial style barrier or terminal strip (and various kinds of jumpers made for that). I think there are shunt jumpers available in larger sizes, though I'm not sure offhand if that's 0.2" between centers but the same 0.025" square post, i.e. 0.1" header with every other pinremoved, or appropriate for the scaled up varieties.Can even use shrouded type connectors, and make plugs with whatever combinations of shunts you need. Probably a bit tedious though.Tim

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 19, 2020, 07:04:38 pm
content: Thanks again for replying. Can you link to some examples? What do you consider to be 'fine' headers? The one I found has a pitch of 2.54 mm, so are you advocating for a larger pitch? What is an industrial style barrier/terminal strip in this case?

author: S. Petrukhin
author_rank: Super Contributor
timestamp: November 20, 2020, 12:40:46 am
content: Quote from: LoveLaika on November 19, 2020, 07:04:38 pmDo you necessarily need high-voltage tracks in the same place as low-voltage ones? Is it not possible to geographically divide the low-voltage and high-voltage parts of the circuit into different sections of the PCB?

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 20, 2020, 03:13:25 pm
content: That's what I'm conceptualizing. Sorry, looking back at my previous posts, I suppose I didn't make it clear.Assuming a 4-layer stackup, I plan to utilize the following:Top: Input and Output Signals, possibly low voltage traces on a Ground PourInner 1: Low voltage traces and possibly a common signal trace on a Ground PourInner 2: Ground PourBottom: High Voltage traces (up to 500 V) on a Ground PourThe bottom layer will connect to the top layer through vias, and I'm using no-fill zones to ensure that there is 3 mm of clearance between the high voltage traces and the ground pour. Again, this is all just conceptual. Things may change, but my original question was about ground pours and high voltage, whether or not to tie the ground pour to the common ground or leave them untied.

author: S. Petrukhin
author_rank: Super Contributor
timestamp: November 20, 2020, 08:49:17 pm
content: Quote from: LoveLaika on November 20, 2020, 03:13:25 pmI use a high voltage film capacitor and a 1210 resistor to connect the common ground circuit to earth.

author: LoveLaika
author_rank: Frequent Contributor
timestamp: November 20, 2020, 09:50:31 pm
content: This begs the question: what is the difference between common ground and earth ground?Ok, common ground is the ground we learn in circuits as a common voltage reference point, and I know that Earth Ground is a thing like in AC circuits (with hot/neutral/ground), but I'm unfamiliar with the differences between the two. Why not just connect them together?

author: retrolefty
author_rank: Super Contributor
timestamp: November 20, 2020, 10:50:57 pm
content: Quote from: LoveLaika on November 20, 2020, 09:50:31 pmThey are usually connected together, the question is where best to make that connection for a given application.

author: S. Petrukhin
author_rank: Super Contributor
timestamp: November 20, 2020, 10:57:24 pm
content: Quote from: LoveLaika on November 20, 2020, 09:50:31 pmThis is a big and tedious theory, I'm not an expert, but will try to explain it based on my knowledge. Maybe I'm wrong about something.If you rigidly ground the common wire of the GND circuit to the PE, all your conductors will become an antenna, and the earth will be a good counterweight to waiting for these intens. In most cases, this will not affect in any way, but it is ugly at least. The flying scheme is better.The resistor is used to allow static charges coming from the atmosphere to drain, for them high resistance is not a hindrance. The capacitor is used to drain high pulses of such charges from touching some objects, including a person - they have a very sharp rise front and a low-capacity accepts them. High-voltage this capacitor due to the fact that static charges have a high voltage, they can break through the low voltage capacitor, it will work as a spark gap once and be damaged.I use this solution for devices running on industrial equipment in open environments with external sensors.