3 Phase Energy Meter PCB Layout Review: Creepage, CT Selection, High Voltage Routing

Dear forum, I would like to ask for help to analyze this layout ive done. Its a 3 phase energy meter and we have a high voltage input 230 AC passing through varistor to protect against voltage surge and there are resistor chain to decrease voltage from 230AC and a voltage divider to condition signal and go to metering chip ... What i already now is that for high voltage designs I need to keep a creepage distance between components pad at least 0.8mm for coated pads, its from IPC 2221 to avoid arcs between then. Another point is avoid routing low voltage signals close to high voltage signals.
I would like to say that I worked with restricted area size, because this board must have this dimensions and have pin headers exactly on that position, because its a module going on another board...
I will have 3 types os current transformer (CT) selection, 5A secondary, 1A secondary and 50mA. As I have CT, after these shunt resistor I will convert current in voltage and I still need to condition signal for energy metering chip. Im ok about hardware project and calculations my doubt is about LAYOUT on this board because thats my second version of this board and I improved so much... Anyway I would like to hear what to improve. I know I have some vias under energy metering chip, its not microcontrooler or processor, only a chip... I placed all decoupler capacitors and components closer to it as well crystal on the same layer as you can see on pictures. I tried do my best with all my experience with restricted size so if someone with more experience here mainly in high voltage boards, let me know where to improve... Ive been following all good hardware practices and high voltage as well but I know as I was saying vias under chip i couldnt avoid, its really tight layout but I thought I did a good job, but as always, its important to hear from experienced hardware engineers...
I know that my track for current transformer isnt wide enough as well, its to withstand 5A but its AC current, not DC current. I have some doubts about it, DC currents and AC current width tracks are different for same voltage, right? I couldnt find any table or calculator like saturn pcb i dont know how to use well or online calculators, but im using 50 mil track for 5A CT.some additional pictures. I placed gnd planes on board. I know I must need gnd plane and high voltages sepparated at least 0.8mm for insulation. As well pin header with 3 pins, gonna have AC voltage thats why I isolated it. However I have a big doubt about current transformer, high current track and gnd plane or vias close to it, i dont know how to proceed very well..

Your creepage and clearance figures are wrong. They need to be higher, if you can't  increase the spacing then you  will need slots milled through the PCB material.This is a highly specialized field, you are working with dangerous voltages, and isolation is critical.I am not clear if this is an engineering exercise only, for personal  interest sake, or it is it planned as a commercial product. If the latter, then the standards testing required to get it to market is time consuming, and very expensive. High voltage testing, EMC, meter standards etc, and the list goes on. In that case, you have to consult with professional standards testing engineers before starting a schematic and PCB layout.If it is for your own use only, I would not risk giving too much advise unless I felt reassured that your engineering background is sound, since there are so many things that can go wrong, some fatally. On the strength of your submission I have some doubts,cheers,Richard

Hi Didan-One trivial note- If you take the trace from J6 to RV2 and move it to the other layer of the board, you can increase your clearances significantly.I  hope you're using 2 ounce or heavier copper.  If those varistors conduct you might have some significant current flowing.-Rick

Richard, thanks for u answer. Based on what my creepage distance are wrong? I disagree with you Im following ipc 2221 and if you can see picture its saying 0.8mm isolation for coated pads, and 1.5mm for uncoated. Im giving 0.9mm for it, what you can argument and not going against well defined rules as ipc 2221 is about that creepage between 0.8mm and 1.5mm for coated and uncoated... Its for commercial buddy and I research a lot about creepage and rules, if you wanna to say its wont going work you need to be more specific because its looking you arent specialist as well saying it... If you wanna more pictures or specific part or measure let me know, lets have a discussion to improve it and how do it

i shouldnt move it, it must be there because i have restrictions and thats all, but thanks to show another way, unfortunately i cant. Well, I will suggest  manufacture this board using 2 ounce 

To clarify- I'm not suggesting moving the trace to the other board- just move it to the other side of the same board.-Rick

Didan,I'd suggest that you look at IEC 61010 or UL 61010. These are safety standards that you will have to meet. I'm not familiar with IPC rules but I believe that they are concerned with minimum clearances for functional insulation. 
Safety standards are higher...

Ok, if what you are saying is right so my 0805 footprint resistor cant be placed there, as resistor chain to drop high voltage and after a voltage divider I get a condition signal for my ADC chip... It doesnt make since considering that I found some commercial boards, 3 phase energy meters using 0805 resistor as well 1206 (which should be safer than 0805) but I found it and it looks work, I couldnt see it but its being selling from them... So it rises a point of dicussion... even if I space my components for 1.5mm lets say this safety distance, what about my 0805 footprints? So, why theres commercial boards from TI, Analog Devices, Maxim, Microchip which you should find 0805... Do you should say me? Im developing my board where I work to work with minimal problems.. I tried 1206 footprint but its too big for that board then I needed to select a 0805 footprint resistor which withstand 400V without break its dieletric, I got it from its datasheet so if my 0805 resistor can lead with 400V over it looks nice to me but it has 0.9mm pads distance while 1206 has 1.5mm pad distance...Link for TI board: http://www.ti.com/lit/an/slaa577g/slaa577g.pdfyou should get BOM from Ti as well... 

For your 0805 footprints, you might be OK as you have them in series so each one is maybe 150V across it and not 400V. But you do need to pay attention to the spacing between each resistor string and between the resistors and everything else.

I will say it again, if you are not an expert in the field of standards testing, then you need an engineer who is to look over your project. I have done standards testing in the past, I worked in a company which use to do this sort of work, and it is complex and expensive to bring a product to market. I have seen some products come back two or three times for trivial reasons, because the engineer designing the boards had not had the experience  and would not take professional advice.It certainly helps to look at other commercial products, but a trivial change can result in a fail.
A bom and a board from an American company that manufactures the chips does not mean that it will pass the various standards required to get it on the market outside America, all they are doing is selling chips.
I wish you well in your enterprise, all the best,Richard

Tips For Improving Your PCB Layout
Make Use Of Top Layout Software
Avoid 90-Degree Angle Traces
Make Use Of A Ground Plane
hope this helps.

good info