4-layer PCB woes

[bean]

I've been getting into 4-layer design over the last few months, sometimes with great success and sometimes with unforeseen complications. The big problem I'm having is with stray DC being present in places it should not be (for example, at inputs and outputs that are DC coupled).

Here's my approach:
Top and bottom layers are signal, 10mil traces. These are 1oz copper.
Two inner layers are VCC and ground pours. These are 1/2oz copper (per the manufacturer spec). I've also done the VCC and ground layers without a pour and using 24mil trace widths. Neither method seems to solve the issue.

My trace layouts seem good (to me) but in areas where I have unwanted DC I'm reading high levels of resistance b/w signal and VCC (on the order of 20-40 MOhm). For example, I have a board that had about 3v on the input pad. Closest DC source is about 10mm away. I generally keep signal and VCC traces @ 90 degrees when they overlap but in this case I had about 1mm of parallel overlay b/w signal and VCC (so that would be top layer and first inner layer). Could that be enough to cause the problem?

I'm more inclined to think this is a result of design flaws on my part rather than a manufacturing error. Maybe I just don't grasp the proper way to do 4 layers. Some work perfectly, some don't. Should I also do ground pours on the top and bottom signal layers?

Anyway, any feedback is appreciated.

Here's an example: this area is tight some some of the routing isn't ideal. I'm picking up DC on all the input/output and Bypass pads, each of which should be 0vDC.

[amptramp]

If you are getting unwanted voltages from another layer, the problem is either the substrate fibreglass has inadequate resistance, inadequate etch time has left some copper where it should not be or the vias between layers are too close to the planes on the other layers.  The layout does not appear to have a design problem so the PCB processing is likely to be the problem.

[Ice-9]

I always use top layer as a signal layer, first inner layer as ground plane, second inner layer as power planes (mulitple voltages) and bottom layer is another signal layer.  I have found that depending on the PCB fab you need to pay attention as some do not offer blind or burried vias which would be a problem if any vias overlap other layers. This was my very first 4 layer failure.

Which fabrication firm did you use ?

[Processaurus]

Silly question, you use the common 1M+ resistors on the input and output of the effect to drain the coupling caps? Without them they'll leak and slowly charge up.

Do you have a bare board you can do an electrical check on, make sure your outputs are an open circuit with vcc and ground?

[Rob Strand]

If you are getting unwanted voltages from another layer, the problem is either the substrate fibreglass has inadequate resistance, inadequate etch time has left some copper where it should not be or the vias between layers are too close to the planes on the other layers.  The layout does not appear to have a design problem so the PCB processing is likely to be the problem.

or an issue with cleaning.

I'm more inclined to think this is a result of design flaws on my part rather than a manufacturing error. Maybe I just don't grasp the proper way to do 4 layers. Some work perfectly, some don't. Should I also do ground pours on the top and bottom signal layers?

The manufacturers usually provide design rules they can meet.   You should only blame your boards if the boards go outside of the manufacturers design rules.   If your boards are within their rules then perhaps they are have production problems.  In this case it's best to ask the manufacturer they a generally quite helpful sorting out production issues.  These days PCB manufacturers can routinely produce very fine structures.    However you have to expect some of the lower cost manufacturers might be not *really* be able to meet their own design rules ever batch.   

Where you want guarantees (perhaps better said as higher confidence) you need to use UL certified manufacturers.   At least you can have some confidence they can build boards to meet their own specifications.  If look at professional products the PCBs are often marked an an E number E.   Normally the customer requests some form of bare-board testing.   Obviously you pay for these services.

https://www.ul.com/services/pcb-compliance-and-regulatory-safety-testing
https://www.raypcb.com/ul-pcb-marking/

Regardless of the manufacturer the best plan is not to push your luck.    If you don't need to cramp things in don't do it.   That's going to avoid problems, even when things go bung on small scale at the PCB manufacturers!   On a few occasions I've had shorts on PCBs from UL certified manufacturers - shit happens.

[Processaurus]

Not to do with your issue, but the internal planes shouldn't be a problem, as long as the vias have a reasonable clearance rule and thermal relief where the thru hole components get connected to a plane. I'd recommend them unless you have a specific reason you don't want them. If routing sensitive grounds you can do a polygon/pour cutout to separate areas and star ground them, like a digital/analog ground. There may even be a way in your software to do a separate AGND and a DGND and do a net tie back at the power input. Overkill for analog pedals but good skills to have. If not using pours it is nice to go fat with the ground and power traces, like 50 mil/30 mil respectively, especially on an internal layer with the thinner copper.

Your board picture looks very conservative/doable for modern pcb manufacturing. 4PCB/Advanced Circuits has a free design rule check on their website for gerbers if your ecad program doesn't have one built in, or if you're concerned one of your design rules (like one of the minimum clearance rules) are set wrong. 

[Processaurus]

or an issue with cleaning.

+1

[bean]

Which fabrication firm did you use ?

JLCPCB. I've had nothing but success with 2 layer designs from them for a few years. But, several suspect 4-layer boards in the past few months.

Silly question, you use the common 1M+ resistors on the input and output of the effect to drain the coupling caps? Without them they'll leak and slowly charge up.

Do you have a bare board you can do an electrical check on, make sure your outputs are an open circuit with vcc and ground?

Not silly at all in this case. It happens to be buffered bypass so there is no input pulldown. I've never had an issue with lack of pulldown on a 2-layer board causing extraneous voltages but I can certainly check to see if it makes a difference. I do have bare boards so I will try some checks for open circuit. TYVM.

Still working through some of the other responses here. Thanks...these are really helpful.

[Ice-9]

I use JLCPCB for 4 layer board and have not had any issues so far (fingers crossed) but I wil say they cannot do hidden or blind vias, so when placing vias you have to make sure that nothing on the other layers will be caught out. Obviously not your problem but just a heads up for anyone working on 4+  layers.

[bean]

Just checking back in to say thank you to everyone who provided feedback. I've confirmed issues across 4 or 5 different 4-layer PCBs and I'm convinced now it's a manufacturing related issue. So, I plan on re-running some of those through a different manufacturer to confirm.

I also plan on contacting JLCPCB to let them know the situation I've experienced. I can write off the expense of failed boards due to the nature of my business but I know a lot of other DIY'ers use them so it would be nice if we all could avoid any future issues.

[phasetrans]

...I also plan on contacting JLCPCB to let them know the situation I've experienced. I can write off the expense of failed boards due to the nature of my business but I know a lot of other DIY'ers use them so it would be nice if we all could avoid any future issues.

Bean, what was the finish on the problem boards? ENIG HASL?

My opinion has PCBCart as the best of the Shenzhen board houses. They have quick turn and full panels. Definitely more expensive than JLC for simple HASL, but very competitive for ENIG, any sort of stack up, and panels. They can also do IPC1, big stackups, controlled impedance, iso 13485, etc.

I have a day job co-worker that likes allpcb for prototypes. Also in China, but not in Guangdong.

Stateside OSHpark for board and MacroFAB for PCBAs. The latter is surprisingly competitive with offshore as long as you understand that there's NRE for the first run, and you should make everything in panel quantities. Slick tool for BOM and board review.

[bean]

So, I have to take back pretty much all of my previous conclusions. The problem appears not to be in my layouts or with the manufacturing but in the actual file setup. I had the incorrect settings on the layer stackup and thicknesses. It's not something I ever had to pay attention to before and I did not have due diligence when I started working on 4-layer designs. A very big mistake but at least I know how to move forward. Luckily some of the other designs I did were not impacted.

[Chillums]

Brian, I'm just starting to dive into 4 layer boards myself.  Do you mind shedding a little more light on what settings caused the problem, and what you had to do in order to fix it?   I'm also using JLC so any insight would be appreciated.  Thanks man!!

PS. Do you use EasyEDA for the schematic/board design or do you use different software?

[pinkjimiphoton]

could it be an inductive or capacitive coupling ? weird stuff happens sometimes.
back when i was still building commercial shit for that dweeb, i noticed the handmade on vero builds sounded way better than the pcb ones, the same components from the same bags had noticeable differences between the two styles of builds.
so noticeable, i even worked up a FAKE pcb "veroboard" that had all the same exact cuts, rails, and jumpers to expedite making the actual "boutique" ones. <i'm sure he's appropriated that without my permission by now, as i was fool enough to send him the idea> my logic being that it should, if made by a fab house to be the same as the vero but pre-cut, sound identical. never personally got that far with the idea, but i guess i should draw something like that up and post it.
but i digress, the point is, the only thing that could have really affected the tonal change between the boards that i could see would have been the stray capacitances from unterminated rails and shit. all those little bits of capacitance and resistance do seem to matter in some circuits,
and you can definitely get weird magnetic fields and inductances... thats why sometimes you have to clock transformers certain ways, as an example, to keep down hum and parasitics and stuff...
maybe your prob with that many boards is a problem like what i described? two like units can exhibit some inductance i'd imagine if proximity is close.. or capacitance.

WAYYYYYYYYYYYYYYYYY above my paygrade....

[MrStab]

Bet you could've done it on a 2-layer board with 1/8W resistors, but that's just my optimistic demeanour.