AC mains on a PCB ?

Ooops - looks like I accidentally hit the wrong reply button before...

On 03/09/16 14:57, George Thomas wrote:

A total newbie to eagle design and PCB fab. So plase bear with on my

silly questions, trying to learn.

 

I have pcb that is schematically completed with the layout. Before i

start the fabrication process i need some expert advise if the

components placed and the wires routed are ok for the ac mains and the

others. The load here will be a transformer. The ac mains are 240VAC and

all works well as designed in the schematic on a bread broad except for

the load for which MOC3023 is yet to arrive from where i've ordered.

You have a lot of traces running unnecessarily close to each other and

to pads. That's fine to low voltage stuff but undesirable when high

voltages are present.

Your placement of parts results in quite a few traces being quite long.

That's undesirable in all domains. I particularly note that the trace

from C7 to R20/21 goes all around the houses, when a simple rotation of

C7 could reduce it to nothing.

I don't know how much current that BTA08 is expected to drive, but the

text describing the board as a "spot welder microcontroller" hints that

you might be looking at several amps. If so, your traces look rather

thin to me, especially given how long they are.

Thanks a lot to take the effort to correct me.

I've removed C7 and R21 which are actually used to protect the optocoupler but i don't see they being necessary here and i have rearranged the the remaining too.

Thanks for your help Robert.

Yes I did change them, the earlier pin spacing was a close. I've changed the locations of the Transformer and reduced the track size of the other components (would that be ideal here as there is not current flowing through them). I've also removed the set of resistors and replaced it with just one and connected to ground such that all the LEDs are grounded via this resistor. No two LEDs would light up simultaneously, tested on the breadboard and that worked well. Hoping this would be a better layout.

On 05/09/16 11:56, George Thomas wrote:

Thanks for your help Robert.

 

Yes I did change them, the earlier pin spacing was a close. I've changed the locations of the Transformer and reduced the track size of the other components (would that be ideal here as there is not current flowing through them). I've also removed the set of resistors and replaced it with just one and connected to ground such that all the LEDs are grounded via this resistor. No two LEDs would light up simultaneously, tested on the breadboard and that worked well. Hoping this would be a better layout.

 

Looks good from the mains side. I can see quite a few opportunities for

improving the low voltage routing and I would probably put all

components at a multiple of 90 degrees rotation (i.e. not like R23 and

IC4) but those are not critical matters. You might want to position IC5

and R20 for maximal clearance between tracks, particularly the T1 gate

track and the one from R19.

Well, after a while, i've managed to move IC5 away from R20, i've also changed the angle for the R23 and IC5 making them more routable during Auto tracking

.

On 05/09/16 23:57, George Thomas wrote:

Well, after a while, i've managed to move IC5 away from R20, i've also changed the angle for the R23 and IC5 making them more routable during Auto tracking

.

 

No, I think you misunderstood. There's no problem with IC5 being close

to R20, there's a problem with the tracks connected to IC5 being close

together. You absolutely don't want them passing between the pins!

Rotate IC5 by 180 degrees and move it left by 0.2" or so. Then rotate

R20 by 180 degrees and move it due south of R22.

IC5 is an optoisolator - its whole purpose is to isolate - so make sure

you maintain an isolation gap across it.

It might help you with getting the separation between mains and low voltage side stuff if you make sure that there is a gap of at least 4.5 mm between mains and low voltage tracks (this is about the separation on the opto isolator package).

Here's a useful guide to this kind of thing:

cache.freescale.com/files/analog/doc/app_note/AN3962.pdf

MK

Thanks mate that was very helpful.

there is a gap of at least 4.5 mm between mains and low voltage tracks (this is about the separation on the opto isolator package).

ah that explains the use of the opto-couplers. I do know that but that made more sense to why they should be separated.:)

so what all the knowledge gain from this post I am guess this the layout should be ok.

Hi George,

It looks like you're really learning a lot with this design and you've had lots of good advice from people on this thread already and the difference between the initial version you posted and this latest version is quite substantial. I do wonder if the placement of the connectors, transformer etc could be rearranged such that the AC traces flow much straighter into the transformer, it's hard to see when you don't have the actual design files to experiment on but I think there is scope for further improvement there. I do also wonder if some of your clearances between conductors, for example around the connectors, are a little small. It might also be worth looking at some reference designs for mains power supply circuits to see how they deal with things like EMI filtering, circuit protection and most importantly safety.

The latter is something I can't stress enough. Do your own research and ensure that your circuit, how it's fitted into your final design, and the system as a whole work together to ensure neither you, nor anybody else, can hurt themselves. Sorry if that sounds a little nannying but as you are new to circuit design and you're jumping straight into a mains powered product it probably should be said. All the advice people can give you here is great but you need to do your own research and ensure that what you finally make is safe and this is entirely your own responsibility.

Best Regards,

Rachael

Looking better on the mains side, although I would still make the tracks to IC 5 thicker - just for durability.

Please review your ground connections, you have some that go through very thin slivers.

Also under the big IC you have floating copper (not connected to anything).

A poor return will make your board bad for EMC also.

Matt.

Am 06.09.2016 um 17:08 schrieb MattyLad:

Looking better on the mains side, although I would still make the tracks to IC 5 thicker - just for durability.

 

Please review your ground connections, you have some that go through very thin slivers.

Also under the big IC you have floating copper (not connected to anything).

A poor return will make your board bad for EMC also.

 

Matt.

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/205233

 

Actually I didn't want to cut in here, but I don't like your AC section

at all.

Distances on terminals are usually just above the minimums.

With your track from transformer pin5 to the AC terminal you lessen the

distance to the second AC terminal pin.

Although the rule says the shorter the better for large currents it

doesn't say to forget the minimum distances

I would:

1. exchange the transformer pins 1/5

2. move R22 right above R20

3. move the triac about half way between the terminals and R22

4. move your tracks straight away from the terminals to get a save

distance before turn towards the triac pins.

5. The trigger line should go a little straight away from the triac

before turning towards the optocoupler.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

so talking about removing floating copper, how can it be done manually ? tried to find it but could not. So I checked the creepage table and to me it was so much unfamiliar terms and French. I managed to learn that 8mm is the minimum distance between AC and DC that needs to be kept. other than that nothing.

Would anyone be knowing a simpler document that I could read.

so talking about removing floating copper, how can it be done manually ? tried to find it but could not. So I checked the creepage table and to me it was so much unfamiliar terms and French. I managed to learn that 8mm is the minimum distance between AC and DC that needs to be kept. other than that nothing.

Would anyone be knowing a simpler document that I could read.

The way to take a little foil off of a pc-board is to slice through it with a sharp, newish pen-knife and then heat up the foil one wants to remove with a soldering iron and scrape it away.  The adhesive usually melts precipitantly.

As an aside, the colored boards have a top anti-static layer, sometimes it is important to scrape this away between op-amp inputs. 

On 06/09/16 17:47, George Thomas wrote:

so talking about removing floating copper, how can it be done manually ? tried to find it but could not.

Assuming you mean how to avoid the unconnected bits on an Eagle board

design, the trick is to turn the "orphans" setting OFF on the polygon.

yea ! your right. That was un-ticked all the while. Ticking it would pour more copper in those empty spaces under IC1.

On 06.09.2016 22:43, George Thomas wrote:

yea ! your right. That was un-ticked all the while. Ticking it would pour more copper in those empty spaces under IC1.

Dont forget those shielded holes in the corner.. I suppose you do want

to put this pcb down in a box? Maybe even shielded metal box?

Interesting project. Without reading it all, I hope you have dimensioned

the AC-LOAD wires for those high currents.

Also, even if this is out of my experience field, I would take an extra

look at this high current current loop. You don't want an EMP generator

For example, I would route the pulsed load pin direct to the AC

input, not passing the transformer first. This will narrow the loop, and

also avoid spikes at the transformer due to voltage loss during current

pulses.

Also, make sure its fire- and explosion-proof in case something should

short circuit, or you get struck by lightning at the AC. I saw someone

mentioning fuse, and I assume you have one at the AC inlet, prior to

entering the pcb.