how wide of traces are necessary for 120V AC, 5amps?

[Michael]

Hi - what size of traces do I need for a 120VAC, 5 amp current? It will
only be about 2cm in length. Also - how far seperated from other traces
will it need to be? Thanks!

 

[Fritz Schlunder]

Hi - what size of traces do I need for a 120VAC, 5 amp current? It will
only be about 2cm in length. Also - how far seperated from other traces
will it need to be? Thanks!

For a PCB track width calculator I recommend this one:

http://www.desmith.net/NMdS/Electronics/TraceWidth.html

The width required mainly depends upon how much temperature rise you are
willing to tolerate and the copper thickness you are using.

I'm not sure how much it needs to be separated from other traces. 120Vac
doesn't start an arc very far (IE: less than 10 mills), however you
generally will want significantly larger spacing for saftey requirements and
otherwise good engineering practice resrictions. Somewhat conductive dirt
could land on your tracks and increase leakage, etc. Perhaps someone else
more familiar can be more precise but I would recommend a good 3mm or
perhaps more.

 

[Michael]

For a PCB track width calculator I recommend this one:

http://www.desmith.net/NMdS/Electronics/TraceWidth.html

The width required mainly depends upon how much temperature rise you
are willing to tolerate and the copper thickness you are using.

I'm not sure how much it needs to be separated from other traces.
120Vac doesn't start an arc very far (IE: less than 10 mills), however
you generally will want significantly larger spacing for saftey
requirements and otherwise good engineering practice resrictions.
Somewhat conductive dirt could land on your tracks and increase
leakage, etc. Perhaps someone else more familiar can be more precise
but I would recommend a good 3mm or perhaps more.

Any idea what the 'standard' copper thickness is? Also - I've seen some
PCBs that had a coating on them - which I would assume is to protect them
from arcing and from things like conductive dust and dirt and such. Is that
something that can be done with a simple spray? Or is that something that
would have to be done profesionally? I'm kinda tempted to just try out a
coat of clear gloss paint on some random circuit...

Michael

 

[Active8]

The rule of thumb is about: 10 mil / per Amp.
So, I would say somewhere between 50 mil and 100 mil.
D = The distance between trace centers.
H = The height of the trace from the ground plane.
%crosstalk = 1/1 + ((D/H) * 2) * 100

Crosstalk and creepage ain't the same thing. Why would you worry
about crosstalk on an AC line input unless it was a carrier current
modem?

There's a different crosstalk eq and lots of other info at UltraCAD
Design, Inc's site - what ever the URL is.

<snip illegible image>

 

[Active8]

Crosstalk and creepage ain't the same thing. Why would you worry
about crosstalk on an AC line input unless it was a carrier current
modem?

*other signal* of course, duh, solly.

 

[ånønÿmøu§]

Also - how far seperated from other traces
will it need to be? Thanks!

With a 1oz copper board. Say, 50 to 100 mil trace width.
Double side 0.64" thick board. To insure a crosstalk figure
of >7% you'll need something like 250 mil separation.

 

[Active8]

Hi - what size of traces do I need for a 120VAC, 5 amp current? It will
only be about 2cm in length. Also - how far seperated from other traces
will it need to be? Thanks!

BEsides UltraCAD in my other reply. There's www.pcbstandards.com

One thing you can be sure of is that a PC mount AC connector will
have the right separation as will a bridge rectifier or transformer
rated for that voltage, so you'd run the traces parallel up to the
input and route inward, perhaps.

The current loop the AC circuit forms is one area you don't want to
route signal traces especially high impedance inputs. That UltraCAD
paper on crosstalk tells the rest of the story. You'll probably
have your power AC supply circuitry in one area, your DC side (?)
on the other side of a rectifier, and your signals elsewhere, so I
wouldn't stress over crosstalk too much.

Why is my Printed Circuit Hdbk always AWOL when I need it?

From der Bible:

for DC or peak AC voltage on an uncoated board at sea level through
10,000 ft.

for 0-150 V -- 0.025 in. minimum spacing. High humidity and/or
contamination will foul this up.

Whew, I'm finding more charts and calculators than I can shake a
tree at - all swiped off the web.

So what's your copper weight and tolerable temp rise? 0.07 in. is
all you need for 5A and 20 deg C temp rise on 1oz copper per R.A.
Gerhold im der Bible. That's 100sq mil at 0.0014 in thickness,
roughly.

The calc at the link provided says the same thing. That's ANSI, so
it says. And it says:

***
The values calculated here compare very closely with those derived
by the UltraCAD PCBTEMP utility.
***

Imagine that. Another plug for UltraCAD.

I don't know what UL says Copy.

Considering your connectors or whatever are going to have spacing
and leads, a 0.1 in track into the doughnut is about right. You
could go more.

Conformal coating. Comes in a variety of flavors and dielectric
strengths. Prevents corrosion from salt air and all kinds of good
stuff. It's not soldermask and it's not any old paint but it might
not be too far off.

Another trick to prevent arcing when you get into the kVs is to
route a hole in the board under components like diodes that have
high reverse voltage on them so the board doesn't contribute to
arcing.

 

[Fritz Schlunder]

Any idea what the 'standard' copper thickness is? Also - I've seen some
PCBs that had a coating on them - which I would assume is to protect them
from arcing and from things like conductive dust and dirt and such. Is that
something that can be done with a simple spray? Or is that something that
would have to be done profesionally? I'm kinda tempted to just try out a
coat of clear gloss paint on some random circuit...

Michael

By far the most common copper thickness is one ounce (1 oz.). This seems
like a rather strange unit of measure for thickness, and it is. It means
that one ounce of copper metal has been deposited evenly onto a surface of 1
square foot. This is a very unintuitive measurement in my mind, but that is
what we use. One ounce copper translates to a copper thickness of about 1.4
mills. 2 ounce copper is twice as thick, 4 ounce copper four times, etc.
Two ounce copper is sometimes used on boards that handle significant amounts
of power/current, but other thicker sizes are rarely used except sometimes
for special requirements in power electronics. Sometimes they use really
thick copper to make windings of really low profile high frequency
transformers.

They do make some spray on substances that are supposed to improve the
electrical peformance of the board surface. I've got some stuff by Tech
Spray "Fine-L-Kote AR" conformal coating in a spray can that claims to make
your circuit surface more rugged while having a strong dielectric strength.
My impression is a real professional solder mask is really quite a bit
better than this stuff.

 

[Tony Williams]

Hi - what size of traces do I need for a 120VAC, 5 amp current?

Your traces have to be big enough to survive the
short-circuit fault current... otherwise they
themselves become the fuses.

A good way to duck most problems is to plant pads as
close as possible to the i/o connection points and
do the mains wiring in insulated solid-gauge links.

 

[Klaus Vestergaard Kragelund]

Crosstalk and creepage ain't the same thing. Why would you worry
about crosstalk on an AC line input unless it was a carrier current
modem?

To reduce coupling from the traces after the RFI filter to the input of the
RFI.....

Cheers

Klaus

 

[mike]

Hi - what size of traces do I need for a 120VAC, 5 amp current? It will
only be about 2cm in length. Also - how far seperated from other traces
will it need to be? Thanks!

Call up your country's equivalent of Underwriters Laboratories.
In fact call up every country where you will ever use the thing.
There's a minimum spec on spacing for mains traces. Do AT LEAST
that much. Not knowing where you are, guesses would be just guesses.
Then call up your board house to get the worst case
resistivity number for the process you'll be using. Assuming you have
a fuse, the fusing current of the traces won't be an issue. Just
calculate the temperature rise and set the trace width to keep
it where you want it. One reliability problem I see a lot in mains
wiring is crystalization of the solder where the wire or pin enters
the hole in the board. Make the hole as small as you can get away
with given the tolerances of the house that stuffs the boards.
Lower temperature rise reduces this problem.
This is less a problem with thru-hole plated boards. Rigid mounting
of connectors is better than handling all the stress thru the
solder joints.

mike
--
Return address is VALID.
Bunch of stuff For Sale and Wanted at the link below.
Toshiba & Compaq LiIon Batteries, Test Equipment
Honda CB-125S $800 in PDX
TEK Sampling Sweep Plugin and RM564
Tek 2465 $800, ham radio, 30pS pulser
Tektronix Concept Books, spot welding head...
http://www.geocities.com/SiliconValley/Monitor/4710/

 

[Michael]

Call up your country's equivalent of Underwriters Laboratories.
In fact call up every country where you will ever use the thing.
There's a minimum spec on spacing for mains traces. Do AT LEAST
that much. Not knowing where you are, guesses would be just guesses.
Then call up your board house to get the worst case
resistivity number for the process you'll be using. Assuming you have
a fuse, the fusing current of the traces won't be an issue. Just
calculate the temperature rise and set the trace width to keep
it where you want it. One reliability problem I see a lot in mains
wiring is crystalization of the solder where the wire or pin enters
the hole in the board. Make the hole as small as you can get away
with given the tolerances of the house that stuffs the boards.
Lower temperature rise reduces this problem.
This is less a problem with thru-hole plated boards. Rigid mounting
of connectors is better than handling all the stress thru the
solder joints.

mike

ah - I'm probably milling the boards myself on a cnc machine. Either that
or I may end up just etching them myself. Depends on if I have to resort to
using any surface mount parts. I'm in the great US of A.

Michael

 

[John Smith]

Call up your country's equivalent of Underwriters Laboratories.
In fact call up every country where you will ever use the thing.
There's a minimum spec on spacing for mains traces. Do AT LEAST
that much. Not knowing where you are, guesses would be just guesses.
Then call up your board house to get the worst case
resistivity number for the process you'll be using. Assuming you have
a fuse, the fusing current of the traces won't be an issue. Just
calculate the temperature rise and set the trace width to keep
it where you want it. One reliability problem I see a lot in mains
wiring is crystalization of the solder where the wire or pin enters
the hole in the board. Make the hole as small as you can get away
with given the tolerances of the house that stuffs the boards.
Lower temperature rise reduces this problem.
This is less a problem with thru-hole plated boards. Rigid mounting
of connectors is better than handling all the stress thru the
solder joints.

mike
--

Excellent advice, Mike.

In addition, experience has taught me not to rely on solder mask for
insulation and protection from surface creepage. The best advice is to
comply with UL requirements and then use a conformal coating for hostile
environments.

John

 

[Michael]

Excellent advice, Mike.

In addition, experience has taught me not to rely on solder mask for
insulation and protection from surface creepage. The best advice is to
comply with UL requirements and then use a conformal coating for
hostile environments.

John

Where would you buy such a coating? Or does it have to be done
profesionally by a PCB etching company?

 

[Richard Henry]

Where would you buy such a coating? Or does it have to be done
profesionally by a PCB etching company?

http://www.humiseal.com/protect/guide.htm

 

[Active8]

To reduce coupling from the traces after the RFI filter to the input of the
RFI.....

Yeah. To do otherwise would be like pissing in the wind, eh?

Cheers

Klaus

Another good reason. That must be why the output is on the opposite
side of the input, not that a board designer would catch that.

 

[Mac]

Hi - what size of traces do I need for a 120VAC, 5 amp current? It will
only be about 2cm in length. Also - how far seperated from other traces
will it need to be? Thanks!

Does this board need to satisfy UL requirements? I recently read somewhere
that UL won't approve a board with mains traces on it unless the traces
are covered with a fire-proof, insulating material such as polycarbonate.

If UL approval is required, you may want to look into this sooner rather
than later.

Mac

 

[John Smith]

Does this board need to satisfy UL requirements? I recently read somewhere
that UL won't approve a board with mains traces on it unless the traces
are covered with a fire-proof, insulating material such as polycarbonate.

If UL approval is required, you may want to look into this sooner rather
than later.

Mac

That may be true, Mac. But, if you design UL now, there may be less to do
later. Lots of times they (the ones who have the say-so) say approval isn't
necessary, then sales finds out the competition is UL approved and the
crunch comes to get it for your own product.

Besides, using UL requirements for spacing seems to me to be a good design
starting point.

My 2 cents.

John

 

[John Fields]

Does this board need to satisfy UL requirements? I recently read somewhere
that UL won't approve a board with mains traces on it unless the traces
are covered with a fire-proof, insulating material such as polycarbonate.

If UL approval is required, you may want to look into this sooner rather
than later.

 

[Michael]

Does this board need to satisfy UL requirements? I recently read
somewhere that UL won't approve a board with mains traces on it unless
the traces are covered with a fire-proof, insulating material such as
polycarbonate.

If UL approval is required, you may want to look into this sooner
rather than later.

Mac

I'm making a total of one of these No UL approval needed!