Post by thread:[EE]: Creepage, clearance and track width

Hi guys, Does anyone know of any good references or rules-of-thumb for creepage, clearance and track width when designing high-voltage/high-current kit? With the parts I've managed to find, at least two PCBs in the mini-oven will need to operate at mains potential -- the power supply and the power-switching for the heating elements. There will be about half a dozen tracks on the switch board running at mains potential, and two on the power supply board. What I need to know is: - How thick these tracks need to be to carry 1650W - Same again for about 15W (the PSU uses a 6VA transformer -- "double it and add a bit") - How much distance I need to have between live and either neutral or a switched HV track. I've had a play with a few creepage/clearance calculators, which suggest that I need a minimum 0.1in gap between L and N at ~300V. So if I was to use 100mil (0.1in) tracks, those tracks would have to be placed on a 200mil grid (assuming they were completely straight) in order to meet that spec. This is based on the output from <http://www.creepage.com/> but other calculators seem to come up with similar results. What I haven't managed to find yet are any guidelines on the required track width for carrying, say, 1650W at 240V (about 7A)... Can anyone suggest any rules of thumb for this? The PCB blanks I'm using are 1oz single-sided, FR4 laminate. If anyone wants to go looking up the datasheet, they're Farnell part number 320-4911, "FR4 composite, pre-sensitised PCB laminate, Eurocard size, single-sided". As this is a one-off, tinning the high current tracks, or soldering bits of wire to them to increase the thickness (and thus the track area and current handling capacity) is also an option, if it makes things significantly easier. I've seen this done in SMPSUs, if it works for them... *shrug* Thanks, -- Phil. spam_OUTpiclistTakeThisOuTphilpem.me.uk http://www.philpem.me.uk/

Philip Pemberton escreveu: > Hi guys, > Does anyone know of any good references or rules-of-thumb for > creepage, clearance and track width when designing > high-voltage/high-current kit? > > With the parts I've managed to find, at least two PCBs in the > mini-oven will need to operate at mains potential -- the power supply > and the power-switching for the heating elements. There will be about > half a dozen tracks on the switch board running at mains potential, and > two on the power supply board. > > What I need to know is: > - How thick these tracks need to be to carry 1650W > Both thickness and width are important. The track width depends on the copper thickness, maximum current (and thus of the voltage if you are speaking of power), track length, maximum allowable loss in the tracks (power/voltage drop) and the maximum allowable temperature raise of the tracks. There is a graphical table used to calculate such things. > - Same again for about 15W (the PSU uses a 6VA transformer -- "double > it and add a bit") > - How much distance I need to have between live and either neutral or > a switched HV track. > There is an IEC norm that deals with this. If I recall it correctly, the tracks must be kept away 8mm for 220V and 4mm for 110V before the current passes some sort of current-limiting or protection device. > I've had a play with a few creepage/clearance calculators, which suggest > that I need a minimum 0.1in gap between L and N at ~300V. So if I was to > use 100mil (0.1in) tracks, those tracks would have to be placed on a > 200mil grid (assuming they were completely straight) in order to meet > that spec. This is based on the output from <http://www.creepage.com/> > but other calculators seem to come up with similar results. > I think you may need 8mm or more between mains tracks. The distance from mains to low voltage tracks may be even larger. > What I haven't managed to find yet are any guidelines on the required > track width for carrying, say, 1650W at 240V (about 7A)... Can anyone > suggest any rules of thumb for this? > Get a copy of the graphical table calculator (I don't know how it is called in English :). Board manufacturers can give you some. > The PCB blanks I'm using are 1oz single-sided, FR4 laminate. If anyone > So you track thickness is already known and fixed. {Quote hidden}> wants to go looking up the datasheet, they're Farnell part number > 320-4911, "FR4 composite, pre-sensitised PCB laminate, Eurocard size, > single-sided". > > As this is a one-off, tinning the high current tracks, or soldering bits > of wire to them to increase the thickness (and thus the track area and > current handling capacity) is also an option, if it makes things > significantly easier. I've seen this done in SMPSUs, if it works for > them... *shrug* > > Thanks, > > ------------------------------------------------------------------------ > > > No virus found in this incoming message. > Checked by AVG - http://www.avg.com > Version: 8.5.409 / Virus Database: 270.13.89/2359 - Release Date: 09/10/09 05:50:00 > > __________________________________________________ Faça ligações para outros computadores com o novo Yahoo! Messenger http://br.beta.messenger.yahoo.com/

Isaac Marino Bavaresco wrote: > There is an IEC norm that deals with this. If I recall it correctly, the > tracks must be kept away 8mm for 220V and 4mm for 110V before the > current passes some sort of current-limiting or protection device. The power input is pretty well protected -- there's a 10A fuse built in to the IEC socket, and a 500mA fuse on the primary side of the power supply transformer. > I think you may need 8mm or more between mains tracks. The distance from > mains to low voltage tracks may be even larger. I've (finally) found the section on PCB design in AoE -- page 841 in the Second Edition. 10A in a 0.170" wide track on FR4 board with 2oz copper will cause a 10C temperature rise. The same current in a 0.080" wide track will cause a 30C temperature rise. According to the text, "for other copper thicknesses, just scale the widths accordingly." So double the numbers then (10C rise, 10A, 1oz = 0.340"). For half an amp the numbers are a little more reasonable.. 0.008" for a 10C rise. That's less than my standard track size (15 mil). For high-voltage stuff: PC runs with high voltage need correspondingly wider spacing -- a good rule is 5 volts per mil (0.001"). So the 100mil (2.54mm) figure is probably about right. The off-board connectors I'm using (5.08mm pitch PCB mount terminal blocks) are rated to 600V, which seems to add further value to the track-to-track spacings I've found. The solder pins are, however, rather thin. Thin enough to make me wonder if the manufacturer is bluffing about the 10A current rating. > Get a copy of the graphical table calculator (I don't know how it is > called in English :). Board manufacturers can give you some. > >> The PCB blanks I'm using are 1oz single-sided, FR4 laminate. If anyone >> > > So you track thickness is already known and fixed. .. But I can always increase it if necessary -- PC power supplies often have thick layers of solder applied to certain tracks on the PCBs (usually in the mains and HV-DC sections) to boost the power handling capacity of said tracks. It's a hack, but if it works for the PCB manufacturers.. why not? -- Phil. .....piclistKILLspam@spam@philpem.me.uk http://www.philpem.me.uk/

Marcel Duchamp escreveu: > Philip Pemberton wrote: > >> .. But I can always increase it if necessary -- PC power supplies often >> have thick layers of solder applied to certain tracks on the PCBs >> (usually in the mains and HV-DC sections) to boost the power handling >> capacity of said tracks. >> >> It's a hack, but if it works for the PCB manufacturers.. why not? >> >> > > Note that 63/37 eutectic solder resistance = 11.5 times copper > resistance. It's hard to see how thick additions of solder would boost > the power handling capacity. > Assuming that the copper thickness is around 0.05mm, it would be easy to add 0.55mm of solder and double the current-carrying capability. __________________________________________________ Faça ligações para outros computadores com o novo Yahoo! Messenger http://br.beta.messenger.yahoo.com/

Marcel Duchamp wrote: > Note that 63/37 eutectic solder resistance = 11.5 times copper > resistance. It's hard to see how thick additions of solder would > boost the power handling capacity. Actually it's not hard at all. The basic "1 ounce" copper thickness is 1.4 mil. There could easily be 40 mils (1mm) of solder on top of the copper, for more than 50x peak thickness. Even if the average solder thickness is only 32 mil (820um), that's still 1/3 the trace resistance according to your figures. ******************************************************************** Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products (978) 742-9014. Gold level PIC consultants since 2000.

Or you can solder tinned copper wire to the bare tracks. (or even copper strip etched or bent to the approximate track shape.) RP 2009/9/11 Isaac Marino Bavaresco <isaacbavarescoKILLspamyahoo.com.br>: {Quote hidden}> Marcel Duchamp escreveu: >> Philip Pemberton wrote: >> >>> .. But I can always increase it if necessary -- PC power supplies often >>> have thick layers of solder applied to certain tracks on the PCBs >>> (usually in the mains and HV-DC sections) to boost the power handling >>> capacity of said tracks. >>> >>> It's a hack, but if it works for the PCB manufacturers.. why not? >>> >>> >> >> Note that 63/37 eutectic solder resistance = 11.5 times copper >> resistance. It's hard to see how thick additions of solder would boost >> the power handling capacity. >> > > Assuming that the copper thickness is around 0.05mm, it would be easy to > add 0.55mm of solder and double the current-carrying capability. > > __________________________________________________ > Faça ligações para outros computadores com o novo Yahoo! Messenger > http://br.beta.messenger.yahoo.com/ > >

On Thu, 10 Sep 2009 17:43:15 +0100, Philip Pemberton wrote: > I've (finally) found the section on PCB design in AoE -- page 841 in the > Second Edition. 10A in a 0.170" wide track on FR4 board with 2oz copper > will cause a 10C temperature rise. The same current in a 0.080" wide > track will cause a 30C temperature rise. According to the text, "for > other copper thicknesses, just scale the widths accordingly." So double > the numbers then (10C rise, 10A, 1oz = 0.340"). There are a few sections in 'PCB Design Tutorial' by David L Jones that give some basic tables for track widths, clearances and rules of thumb (including some pertaining to altitude). You can grab a copy from: http://www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf Personally I think it's an excellent document on the whole; there's enough to get started with PCBs and also to use as a reference - a lot of info and advice packed into one place. I would've mentioned it earlier but I thought you were after something more substantial/formal - but IIRC it has a bit more detail (tables) than the AoE treatment, although it does make a few mentions of 'the relevant legal standards' but unfortunately gives no reference/source. Hope this helps anyway. Regards, Pete Restall

Peter Restall wrote: > www.alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf [...] > I would've mentioned it earlier but I thought you were after something more > substantial/formal - but IIRC it has a bit more detail (tables) than the AoE > treatment, although it does make a few mentions of 'the relevant legal > standards' but unfortunately gives no reference/source. Yeah, I'd have preferred a more "concrete" reference, but nearly everything I've found seems to say the same thing. It looks like IPC-2221A is the "universal reference" for this sort of thing, but I will be keeping a copy of the PCB tutorial on my bookshelf. Now I just need to rebuild the horrendous component libraries that come with EAGLE and KiCAD... Then I might actually be able to design the AC board. The controller board (by comparison) should be considerably easier to design... Thanks again, guys. -- Phil. .....piclistKILLspam.....philpem.me.uk http://www.philpem.me.uk/

Philip Pemberton wrote: > Now I just need to rebuild the horrendous component libraries that > come with EAGLE and KiCAD... Yeah, the part libraries supplied with Eagle suck. The board footprints don't seem to follow consistant conventions, the silkscreen is often sloppy, and the schematic symbols appear optimized for the time it took to throw them together instead of for readability in the schematic. Long ago when I first started using Eagle I used parts from their library because making all my own seemed so overwhelming. That got me into trouble, so I haven't used the Cadsoft libraries since. It's really not that hard to make your own as it may seem when you are starting out. It also allows you to stick to conventions about parts that help with automating things later. For example, all my parts have their designators in the tDocu or bDocu layers in small text. These are used only in the board drawing and helps the manufacturer find a part regardless of if its designator made it to the silkscreen layer or not. (There is also a ULP for generating a parts index that gives board and schematic coordinates for every part, but that's a independent issue.) Another important part of my conventions help in automatic BOM generation. If you set all the right attributes, then you can go fully automated from a Eagle board to a Excel BOM with my ULPs and host programs. Take a look at the CSV_BOM and EAGLE_ATTR doc files after installing my Eagle tools release from http://www.embedinc.com/pic/dload.htm. ******************************************************************** Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products (978) 742-9014. Gold level PIC consultants since 2000.