Searching \ for '[EE]: Creepage, clearance and track width' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/index.htm?key=creepage+clearance
Search entire site for: 'Creepage, clearance and track width'.

Exact match. Not showing close matches.
PICList Thread
'[EE]: Creepage, clearance and track width'
2009\09\10@092214 by Philip Pemberton

face
flavicon
face
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_OUTpiclistTakeThisOuTspamphilpem.me.uk
http://www.philpem.me.uk/

2009\09\10@101357 by Isaac Marino Bavaresco

flavicon
face
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}

__________________________________________________
Faça ligações para outros computadores com o novo Yahoo! Messenger
http://br.beta.messenger.yahoo.com/

2009\09\10@124320 by Philip Pemberton

face
flavicon
face
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.
.....piclistKILLspamspam@spam@philpem.me.uk
http://www.philpem.me.uk/

2009\09\10@132238 by Marcel Duchamp

picon face
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.

2009\09\10@134218 by Isaac Marino Bavaresco
flavicon
face
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/

2009\09\10@161144 by olin piclist

face picon face
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.

2009\09\10@162706 by Richard Prosser

picon face
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 <isaacbavarescospamKILLspamyahoo.com.br>:
{Quote hidden}

>

2009\09\11@142545 by Peter Restall

flavicon
face

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

2009\09\11@151218 by Dario Greggio

face picon face
Peter Restall ha scritto:

> 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

Nice and interesting, thank you! :)

Dario

2009\09\12@074953 by Philip Pemberton

face
flavicon
face
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.
.....piclistKILLspamspam.....philpem.me.uk
http://www.philpem.me.uk/

2009\09\12@083715 by olin piclist

face picon face
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.

More... (looser matching)
- Last day of these posts
- In 2009 , 2010 only
- Today
- New search...