Triac track width and clearance advices?

"Hallet" <antoinehallet@yahoo.fr> wrote in message

news:h4k5pf$h9q$1@cheetah.cadsoft.de...

 

What value do you use for track clearance for 220V mains voltages?  Ive

seen 0.75mm (http://www.electronics-project-design.com/PCB-Design.html )

for coated board. But here

(http://www.smpspowersupply.com/ipc2221pcbclearance.html ) the values are

not the same and I dont know what to use? Is bare board for PCB without

parts on it? So do I have to use assembly and external components leads,

uncoated if : the board has a solder resist mask, is populated and if

there is no coating on component leads?

Is the clearance also needed between the components pads (external

diameter to external diameter)? If so, is it possible with a standard

TO-220 package?

 

Take a look at these links:

http://www.smps.us/pcbtracespacing.html

http://www.pcbwizards.com/faq.htm

Related- you can look for 'creepage and clearance distance'

Thank you for your answers.

@jrafetseder

It's a special manufacturing process, it's not a standard technology. For just some board it would cost a lot.

I have tried to bend the triac leads (like some TO-92) in order to respect the 1.5mm clearance, but I think the leads are too small to go trough the PCB. The clearance should be 1.50mm from 301 to 500 AC peak and 0.75mm from 251 to 300 AC peak, so if I have a little less than 1.5mm I suppose it's not a big problem... The TO220 package doesn't seem to be well designed to respect the IPC clearance. 

Can I use a track of 2.54mm wide (small length) to connect to a wider track or polygon?

Thank you.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

a track larger than the pad is not a problem, the pad may get somewhat

hotter than the rest of the track but it's small and attached to a big

track and big component lead that will be most likely hotter than it is.

  the big track improves heat sinking, this only becomes a drawback if

it makes soldering the pad difficult, that's why a polygon will generate

a thermal isolation around the pad.

an 8 amp triac when on will generate about 8 watts, that's a big waste,

consider using some arrangements of low Ron MOSFETS or optical relays to

perform the same task with /way/ less heat. triacs also trigger

unpredictably on inductive line transients, in my experience. you need

to test for this, a good test is to plug in a vacuum cleaner on same

outlet as the DUT and turn it off and see if you don't get transient

conduction in the triac, bet you will

the covered and uncovered specs for track temperature rise refer to the

presence of solder mask which increases heat rise in a trace.

as for isolation, at atmospheric pressure, you don't need much, at low

pressures, 5V will produce corona discharge. route your 220V traces with

user safety (fingers, tools, scope probes) in mind. i would make them

covered with solder mask. to find the minimum clearance, you need to

look up the dielectric strength of air at your ambient temp and

pressure. use the peak voltage of the AC wave. you shouldn't have any

trouble giving yourself a generous safety factor at normal air pressures.

that enough advice for ya?

take a look at this:

http://www.haeusermann.at/2,product/14,HSMtec/15,Hochstrom--und-Waermemanagement-auf-der-Leiterplatte

if it's in german, an english version is available

r

Hallet wrote:

Hi,

 

Im making the layout for a PCB that uses a triac in TO-220 package.

The maximum current in the triac (BTA312Y) is 8 Amp. and the copper

thickness 35m (1 oz/ft^2). What track width would you recommend? Ive

seen calculators on the Internet but they ask the allowable

temperature rise and I dont know what value I can choose. On the

other hand, Ive seen that IPC recommends 220mil for 8 Amp., 10C rise

and 1oz/ft^2 Cu but its very big?

Well, 8A is a lot of current, so it will require a pretty fat trace.  For

temperature rise, what can you tolerate?  If you have a "nice" ambient

environment of, say, 25C, then you might consider a greater PCB trace

temperature rise.  If you allow a 30C temperature rise, then the PCB tracks

near your TRIAC might rise to a temperature of 25C + 30C = 55C.  If your

TRIAC is mounted to the PCB, then its case may also be at 55C (though you

probably have a big heat sink), so you'll have to consider that in your

calculation of junction temperature in the TRIAC.

At a 30C temperature rise, you only need about a 100mil track to carry 8A.

If you can use 2oz copper instead of 1oz, then you can halve the track width

again.

I would use as much copper as possible for conducting the current.  I

generally use polygons to make use of all available space for carrying big

currents -- more copper is better.

What value do you use for track clearance for 220V mains voltages? Ive

seen 0.75mm

(http://www.electronics-project-design.com/PCB-Design.html ) for

coated board. But here

(http://www.smpspowersupply.com/ipc2221pcbclearance.html ) the values

are not the same and I dont know what to use? Is bare board for PCB

without parts on it? So do I have to use assembly and external

components leads, uncoated if : the board has a solder resist mask,

is populated and if there is no coating on component leads? Is the

clearance also needed between the components pads (external diameter

to external diameter)? If so, is it possible with a standard TO-220

package?

Sorry, little experience with 220V clearance requirements.  Maybe somebody

else will comment?

--

Bert Menkveld

If your application has to work in low air pressure, such as in

aviation, then the clearance specs require much wider spacing.  Low

pressure air arcs over much easier than normal pressure air.

Robert Scott

Real-Time Specialties

Ypsilanti, Michigan

Anybody has some advices?

Thank you.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca