Ok I am having a heck of a time routing my board. I am putting alot of parts on a pretty small board. 3 speed switches, power supply, rf chip and an h-bridge on a 3.5" X 1.6" smd two sided pcb.
After doing some reading I am considering adding 2 more layers.
the formula I have decided to use as recommended by the eagle manual is (12+316)
I was thinking 3.3v gnd on one layer (top), 3.3v hot on another layer (2), +115v hot on another layer (3), and Neutral on the bottom layer.
My question is what size isolation layer should I place between the copper layers.
The default Eagle came up with is 1.5mm between 1 and 2, .15mm between 2 and 3, .2mm between 3 and 16.
I realize that this plan may not work. If not please let me know what might help my routing problem.
This plan won't work. Not safely. While the PCB material on its own will probably be an adequate barrier between the 115V and the low-voltage parts, you probably have vias and component legs that go through the board. You need a big isolation gap around those punctures.
The problem with 115V is not really the voltage. The problem is that it's connected to wires outside your building. A nearby lightning strike (on another building) can deliver really frightening voltages into your circuit. At those voltages, air is no longer a perfect insulator. The PCB surface can hold contaminants like fingerprints which will allow high voltage to "track" across the surface into the low-voltage side.
First, does any person ever touch any low voltage component while the circuit is plugged into the mains? If you use mains-rated buttons and the whole thing is tightly locked in a plastic box, then you can consider the entire thing 'live' and don't worry about isolation. Use the Eagle recommendations. If you've got a regular pot or low-voltage switch penetrating the plastic box then you have to apply isolation to make sure that that component can never become live under fault conditions.
If you've decided that you must have people touching the low-voltage side, then you need to partition the PCB into high and low voltage. To prevent tracking, you try to put cutouts in the PCB. If there's no material to hold dust or fingerprints and the gap is wide enough then sparks can't jump the gap. Certain components must cross the gap. The 3.3V power converter, opto-switches or whatever. Always use mains-rated components in those positions. A typical opto might have a "breakdown" voltage in excess of 4000V. That makes it a relatively large device, otherwise the sparks could track around the outside of the case.
If you still need a 4-layer board after all that, then pick a manufacturer (I like OSH Park) and download their board specifications. Making up your own thicknesses is only economic if you're going to build thousands. Otherwise it will cost you more than US$1000 for a one-off stackup.
I have others telling me the same thing. One forum friend has pm's me about not needing snubbers on each switch as long as my triacs are snubberless and my opto's have zero crossing triggers. He indicated that one snubber across the motor should be sufficient for the entire circuit.
This move has eliminated alot of the parts that were causing my routing problems. I only considered this because my manufacture pcbcart.com has an option to choose 2 or 4 layer in their price calculator. My thinking that it should be cost effective.
With your advice and that of others I am going to try to route the board with 2 layers again.
Originally I was just adding copper pour to each side wiring it to 3.3v gnd. Does that sound reasonable?
that is really the only common piece I have to route (goes to each opto) that isn't on the 115V side.
I have 3 airwires not connected and they are all going to GND1 which is my ground plane that is poured on both layers 1 and 16 why aren't they just connecting to that.
Just and FYI I really got more questions then answersm
For pcb manufacturing I use pcbcart.com make sure to choose prototype when getting a quote from their online calculator. prototypes are way cheaper. I believe it's a max of 4 layers the board price - mine is like $35 for 5 boards (5 days to print) you will have like $35 in shipping which is fast in my mind usually about 3 - 4 days from when they indicate they shipped. So for around $70 for a small board you have a prototype in 10 days. I felt that was fair and cheap.
Tom here is a snippet of one of the switches on the board ....
You can't see it here but after much thought and advice from some very smart folks on this forum I am running one snubber between black and white (hot and neutral). The data sheet for the triacs say it's not necessary but due to the type of motor we decided one snubber would be sufficient
Not much to see I am using MOC3162M with zero crossing trigger as the opto
I am using KTR10EZPF3600 360ohm resistors
also a T850-6G snubberless logic level triac
All rated for at least 250VAC of course all are the smd version.
You can't see the net names but this one is switching +115V with the common on the caps pack of the fan and will give me high.
The prototype circuit I built served the same puprpose high on the fan. I used through hole parts and not the smd parts I have designed the board with but the prototype was the same otherwise.
I switched it on and off and let the fan run and I never noticed any heat at all.
My board has an rf-mcu, power supply, 3 speed switches, one light switch and 4 switches set up as an H-Bridge to reverse the fan.
The 115V portion of the board has 15 mill traces and 15mill clearance upgraded from the 12 I believe eagle defaults to
Tom if you are interested in looking at the eagle files I am going to be doing some work this morning adding a hole to mount the board and of course finishing up the air wires that still need routing before creating the gerbers and ordering if you want shoot me a PM and I will give you a link to the files.
mtalent:
hey Morgan (or others) quick question....
refer too following snip .......
I have 3 airwires not connected and they are all going to GND1 which is my ground plane that is poured on both layers 1 and 16 why aren't they just connecting to that.
Any help appreciated
Mark
Without the schematic, I'm not sure what you're trying to achieve here. Normally you name the ground planes GND and then any GND net on the schematic will connect to both. More than one ground is only used if you have a special analog ground or there's a "high voltage" ground which must stay confined to the high voltage area of the board.
Sometimes you get "islands" where the ground plane doesn't connect to itself. In that case, it's often simplest to place a via which will connect the island to the ground plane on the other side. After placing the via, name it GND and it will connect on the next ratsnest command. The next thing to look at is any areas where you can nudge wires over and allow the ground to flow through. There's an obvious candidate in the middle of your picture.
Yes I figured that out this morning fixed it with three well placed via's.
My board only has one ground the reason it is called GND1 is because when I first started I was thinking I would need 2 grounds (this is the first time I've done this). When I discovered I only needed one I just kept the name GND1.
I should give some credit to Raynold too he said the same thing.
Anyhow gerbers are filed with manufacture and in 10 days we can see if it works.
I prototype the whole thing using relays and tested system using esp8266 and mqtt.
Then I built one of the switches with the opto's and triacs and used it to run one setting (high on fan)
I ran that for a while and switched it on and off without problems.
Then built the board using the same switch setup only with 8 switches, 3 for speed control running through caps pack, one for light, 4 for H-Bridge to reverse motor direction.
this entire setup is just proof of concept will only ever be used and handled under experimental conditions by me only.
If I continue with project I plan to build board to UL specs. I have been researching these they don't sound too awfully hard but I will have engineer to help to fine tune equipment.
