looking for input on design

[sphinx]

i am fiddling with a design with 230vac and looking for input on pcb design with that voltage
 track width spacing etc. at this time only the in stage is more or less complete so far.
just need to ad som sort of sockets or gave the solderable for cables as it made now.

its made with altium v16.

p.s.this is only for personal use not any commercial use

made some small update to tracks and moved some components to get better clearance
and other adjustments thats the second url.

[UncleBog]

I've attached a link to the IPC standard that covers track sizes and separation.

[fpgaguy]

take a look here, there some IPC / UL / IEC standards covering that
http://www.smps.us/pcbtracespacing.html
http://dkc1.digikey.com/US/en/TOD/JohansonDielectrics/PCBDesign/High_Voltage_PCB_Design_for_Arc_Prevention.html


or you can google "arc+voltage+pcb"

this will get you spacing data, for width it's a question of current you need

[LzEn]

i am fiddling with a design with 230vac and looking for input on pcb design with that voltage
 track width spacing etc. at this time only the in stage is more or less complete so far.
just need to ad som sort of sockets or gave the solderable for cables as it made now.

its made with altium v16.

p.s.this is only for personal use not any commercial use

made some small update to tracks and moved some components to get better clearance
and other adjustments thats the second url.

You can use http://www.creepage.com/ to calculate the spacing between the tracks based on the voltage. This calculator is based on UL standards.
For the width it is based on the current drawn. Many PCB track width calculators are available on the net.
Saturn Toolkit is a great tool for general PCB calculations you might want to look at. https://www.saturnpcb.com/pcb_toolkit.htm

[sphinx]

i downloaded saturn toolkit and have used it to get help on track width and spacing,i kinda also wanted on the layout itself.
i know layout is personal thing and the way to do it is a personal preference, but input and ideas and experience is allways nice. i am just a novice in this area so get more knowledge is allways a good thing.

[Sideshow Bob]

Have you sourced all the components like the transformers. Also have you given any thoughts about proper cooling?

[sphinx]

the tr4 and the tny267 are not yet sort of checked up so far since i am not too familiar with designing switched power
supply,  the 12 volt output cant be modified changed since its the only use of that dc voltade is only used to delay
the relay to lower the inrush current for all capacitors so that part is not important and can be changed if circuits or
circuit is not available. rest of the components are checked and ok, this might or not be built in real life. if this is built
i will certanly use good cooling with big heatsinks i will try to use 50% more cooling than needed at least i will try to figure
out whats needed at 100% load and add to that so the unit wont be undercooled. and idea would be to add a separate microcontroller or similar for overremperature  and fan spinning to check for faults, but this last also doeas not bother me
because thats simply added at a later stage.

i do this to excersize my brain since i am too early retired from any work i just like to keep head working with either software or this sort of things for interesting ideas/projects i find fun to do/fiddle with.

i checked and the tny277 can be used as replacement with changes since its not pin compatible and maybe component changes so its to look up a transformer and add/edit/change/modify this to schematic and pcb.

[mexpcb]

I was almost going to go and change your layout for you but because you just mention you wanted to do, here are some comments..

1.- You are missing the Footprint for the Bridge

2.- when you have 2 vias or hole to close with a small gap (1~6 mils) and if they are the same net, the Altium Default Rules will not flag those as a DRC, you may need to adjust the rule to include the same net feature or just go ahead and add a fat trace similar of what you did on the NetC2_1

3.- when you have a thru hole component and if that it’s a high current pin or net, please make sure you add some more surrounding vias and add enough copper on top layer and bottom layer, this is because if you just use one via or hole the current will go all the way in the via or hole barrel edges but if you add a plane and more vias it does allow more current to get out on top or the bottom plane (depend on where it gets placed), then the additional vias will help with more current.

4.- if you are going to solder this manually, go ahead and make bigger pads and solder mask openings in all your thru hole components, you may not need thermal ties to this because it will be not to much copper to heat and you will solder this manually, the same comment from before can be added to any pin, this will also help to keep the copper on the board if you need to solder or replace some components.

5.- looks like all the bypass or filtering caps are the same values, you don’t need all of this, maybe even if the Footprint is the same you may need to add different values but the important think here on the layout is to avoid having those finger kind of connections make some straight lines and connect them as its shown on the schematic

6.- I didn’t revise the schematic very well but is resistor R3 correctly connected?

7.- the way you have connected the second Block IC2 its just after the Bridge or transformer (Physical Connections), if you want the good filtering signal in this second and third block you need to get the connection from the last cap after the bridge, because if you just take the connection from the first cap, you will not get the benefits of having the other ones there.
 

i may give you more tips or guides but first let’s see what do you think about my comments or if you have more info about your circuit...

I’m not really familiar with such low frequencies but for any oscillating signal in this case AC, the signals go between the conductors and when you are dealing with this nets on the PCB, just try to keep some kind of parallelism and isolate or keep far the DC signals from the switching signals.

And lastly form another view, if you are worry about having some kind of arcs in your circuit, what I know is that the voltage is what it creates the arcs, and normally when I play with some ESD Test Devices the Voltage needed was too high to get some arcs, so I think in this case if you keep at least like 30~60 mils minimum between the + and – it may be find, let’s see what did you find on the Calculators…

for now, this is a quick reply and i hope it does help.

Regards

[sphinx]

i uploaded updated files and docs. these were done before your comments.

i changed to updated chip thy277 and transformer core footprint. and did some other adjustsments too. the bridge is not missing
i made pads instead so i could place it on a heatsink and use short wires to connect.

about r3 according to schematic its right.

yes the design will be done for manual soldering, i think i will mod the pad at last when its all completed.

i will read thruu what u wrote and try understand/figure out what u mean with it, my head works a sorta slow so it sometimes
takes some time to get it.

and sure i am happy to get pointers/help... that can help me on the way

here are update files and info to download for those who like.

i have updated after reading the so please redownload if u cant download design

[mexpcb]

its a good practice to add Footprints to all the components, attached its an image when i try to transfer the netlist to the board (ECO), some Footprints are missing and some nets of course. i know you will connect them manually but doing thinks manually can lead you sometimes to make mistakes...

also there are some nets unconnected, look at the missing connections image

looks like you will fabricate this at home and you are trying to make all the connections on one layer, this is good but you need to maybe rename the nets to easily identify the type of nets, in example after the AC gets filtered (DC), you could identify the Ground and name it as Ground (in This Case is a switching Signal but it can help you to identify and make better routing) , then on the Layout you will make a Big Copper Areas or at least to help you to isolate the different type of Signals..

if you are able to make two layer Boards it may be better, then you can add each "Reference Ground" on each step just bellow the "Positive" signals on the Top Layer, its like for Pure DC, to make all the Positive Voltages on Top  and a Big Ground underneath on the Bottom Layer, in Your Case you need to be carefully with each step because they are different type of Signals...

The Layout its getting Better and i'm glad to help you in what ever i can...

Regards

[sphinx]

i had the bridge and KAC and KDC in the design only until i figure out how to do it without them since i already added pads for
cables and so can place bridge on a heatsink. all is now connected and modifications made, i think i am now at a point where
i am not really making it so much better.

i attached latest so if you want you can have a peek at it.

i am going to read what said and implement that on the design

i have watched some of fedevels videos and ohther youtube's yo learn on how to do this kinda stuff.

[mexpcb]

Personally Don't waste time looking a Fedevel, he just show you how to use the software, of course its important to know but he does have some bad habits on creating Designs and it looks like he does not have experience creating Real PCB for the industry, maybe at some time he did but looking at the videos for me there are some more important thinks to know when creating PCB's...

This are some Basic Rules and General Knowledge..

Always keep in mind how the current Flow (in theory)

Always know what type of Signals you are routing

for The Power Nets (High Current in Your Design), do use Fat Traces or Planes

for the Signals, always look at the Return Path and place it Close to the Signal Path or in parallel.

always think on how you will be assembling or soldering your parts.

Sometimes do follow the connection as you may drawn the schematic, this is to avoid confusion when you are on the Layout, in example, on the Layout you always see Net Names, and the target is to Connect them, but do it on the way that it does make sense, like one example i give you on the Caps.

for manufacturing purposes, for a non expensive or standard board you can use 12 mils of spaces Copper to Copper, 12 mils of trace widths, 20 mils from Holes to a Different Net, 10 Mils of Annular Ring for Vias and for Thru Hole please make sure you will have enough space for soldering, 20 mils it may be good, or take a caliper and you will get an idea, for solder mask you can use 4 mils of Solder Mask Expansions, something like this, those are not mandatory values but if you will use a fab house, please check with them, all of them have different requirements but in your case the rules i mentioned it will work for you, you can do less in some cases but those will be easy to do by any manufacturer or even if you are doing it at home.

in your case you can make the traces as fat as you can but always please keep in mind the different signals and do not get them so close because they may interact one with the other...

by the way, i'm not against the fedevel guy but do not trust him on all he say, trust me, i have a lot of experience doing PCB for any application you may think, just to give you an idea i have made 50 Layer Boards of 537mm by 457 mm, Control Impedance Traces on (24 layers), Differential Pairs, Length Matching, 8000 Nets in Total, 6233 components, etc.. and a lot more PCB's for +60GHz..

if you could give me the Complete BOM i may be able to Do from scrach and make a video for sonsivri Guys , what do you think? you can use you board but i just want to explain some bad habits even so called profesionals do with schematics and layout, actually i'm creating some videos of how to properlly do a MKR100 Iot Arduino Board on Altium, but this is not completed yet....
 Regards

[sphinx]

i very happy for all your input and i like to learn specially in electronics and coarse fishing those are the 2 of my passions i try to keep alive
i use fishing as a way of relaxation and fun, electronics just because its always been something i really liked to fiddle with and to keep my
head working. i will put all your info in a file and have it as a reference and good things to keep in mind.

i will now work on sorting things up in the pcb like net names and making some ground planes around the IC for cooling.
ans some other finetuning because i now think i have come to the stage where i think i will more mess it up than do any
good.

sadly the only thing i got is that webpage with schematics, and from i so looked at it some components will have to changed
i will need to look and see to what to exchange them with.

regards

[maurer]

mexpcb, can you suggest any reference book for pcb design ?