Reduce PCB size

Hi, I was wondering if anyone could tell me some tips on how to reduce PCB size.

I want to reduce the size by atleast 30% of the attached circuit.

There seems to be a lot of empty space in the bottom left but you can't cut it out because the length of other components are too large. Maybe make Q7 vertical and make the 3 ICs just below Q7 vertical and then reduce the width of the board. Turning DB7 horizontal and moving it so it is just above the large IC to it's left should help reduce board height too.

Use smaller traces to route in between the pins to pull that off and maybe make some traces on the red layer so you can route it under the largest IC so it can connect with DB7.

All that is easier said than done though because of the routing.

If i make Q7 vertical, all the traces will have to come out from the side and then connect with the IC's. That wont reduce width i think. I have attached another image which has a little more space free on board but i still am not able to reduce board width and height

You can see how I have brought things together to gradually reduce the size of the board. Just keep doing this until the board is the required size. The resistors can be stood "on-end."



**broken link removed**

Guess this why they refer to PCB, as 'artwork'... Takes practice, a little talent and skill to pull off.

Well you could obviously switch to SMT components but I assume that's not an option.

It's possible, you may be able to eliminate some of the components, post a schematic and we might be able identfy the redundent components.

I think i can use SMT resistances only. Other components might not be available is that package.

I hope i dont get SMT resistance wattage issue.

Sorry i do not have a schematic. Just used three different circuits into one. Its an electronics Fan dimmer i have been trying to make.

One portion is the Zero crossing detection, one is Controller portion and one is Power Triac portion.

haxan said:

I think i can use SMT resistances only. Other components might not be available is that package.

I hope i dont get SMT resistance wattage issue.

Click to expand...

Use Ohm's law to deturmine that.

Sorry i do not have a schematic. Just used three different circuits into one. Its an electronics Fan dimmer i have been trying to make.

One portion is the Zero crossing detection, one is Controller portion and one is Power Triac portion.

Click to expand...

So does it have mains and separated extra low voltage (i.e. a low voltage DC supply) on the same circuit board?

You should leave adequate spacing between the mains and DC side to ensure protection against electric shock.

The following articles will guide you on this:
**broken link removed**
**broken link removed**

Table IV, in the article gives the creepage distances to fulfil the requirements of basic or supplementary insulation.

You haven't said what the voltage is or what environment your device will be used in. Assuming it's going to be used in an office, home or school then it's pollution category II , most most PCB materials are material group IIIa or IIIb and from table IV the creepage distances for 120V and 230V are 1.5mm and 2.5mm respectively.

Note that the above distances are for basic or supplementary insulation, the DC side needs to be double insulated from the mains so the distances need to be doubled.

Basically, if the mains voltage is 120V you should leave a minimum distance of 3mm between the mains and DC side and if the mains is 230V the minimum distance should be 5mm. Note that this only applies for indoor domestic and office appliances, not equipment designed to be used outdoors or in a factory.

oh wow, Yeah i have both 220V and DC 5V on same PCB. I think the distances are more than 5mm so i guess i am safe for now and i am building it for personal home usage

Here's a site with a calculator for working out the creepage and clearances.

I tried running the calculation for 250V mains (the maximum nominal voltage) and double insulation. The result was 5mm which is to be expected.
WWW.CREEPAGE.COM Welcome!

I know there's no scale or indication of which tracks are which but some of the tracks near the opt-isolators look pretty close. I'd recommend checking them so you can be sure they're >5mm - when mains voltages are concerned it's better to double check and be safe rather than sorry.

yes you are right but the problem is that is the triac's gate trace and the Triac's three terminals are pretty close. There is not much i can do about it The only solution that might be possible be to create my own pads for traics.

You need to understand that, for safety purposes, there are four different class of electrical insulation:

Functional insulation
Only required for correct operation of the device and not protection against electric shock.

If the functional insulation fails, the device will stop working, a fuse may blow but there should be no possibility of the user receiving a shock.

All other types of insulation are important for protection against electric shock, they are as follows:

Basic insulation - stronger than functional insulation and required between earthed metal parts and the mains.

Supplementary insulation -an additional layer of insulation as a backup in case the basic insulation fails.

Reinforced insulation - a very strong layer of insulation designed never to fail.

Double insulation
Can be either:
A layer of basic insulation and reinforced insulation.

Or: a single layer of reinforced insulation

The insulation between the TRIAC's gate and three terminals is classed as functional insulation only and is not protecting the user from electrical shock. The spacing for functional insulation doesn't need to be as large as reinforced or basic insulation which are safety critical.

The 5mm rule only applies to 5V traces and pins running near 230VAC traces and pins.

I've just realised another thing: is the 5V derived from a transformerless power supply?

If so it should be treated with the same respect as mains and the 5mm rule doesn't apply since it is the same as mains, for safety purposes.

I don't have a very good feeling about this, it could be very dangerous.

The power is being driven from same source, one coming directly (220V) and one coming from transformer and then being regulated to 5V using 7805.
Well i guess the only way would be to test it by making PCB.

Just a silly question, would applying solder mask do any good or not.

That sounds much better than a transformerless power supply.

I've read conflicting pieces of information in the article. The calculator seems to spit out much lower figures when set to a coated board but an article I read states that it shouldn't make any difference. My opinion is that a solder resist should improve it a little bit but I'd still try to leave 5mm between mains and DC where ever possible.

To be honest, I can't tell you whether your PCB is safe or not and won't be able to figure it out unless you tell me which tracks are mains and which aren't.

Oh sorry, well the thick traces are mains. The one in my original pcb layout with ~ sign is hot line (phase) and next to it is Neutral (N). Both the thick tracks written next to 1 and 2 are the outputs of 220 going to Fan. The + sign means DC 5V and - means DC Ground.

The 220V when goes to the bridge (circular component) drops voltage very close to 1V (i do not know why) but gives correct Zero crossing values to the two PIC12 Controllers right below the 07 header. These PIC's according to the latched data from 07 header Dim the fan speeds by phase control using triacs and MOC3020's.

The big IC is just a flipflop which takes input from one header and latches it to 07 header.
I hope its a little more clearer now.

I've highlighted all the tracks at mains potential.

First ensure the other tracks have at least 5mm of creepage before you try to shrink it.

Fortunately, it's possible to shrink it even more whilst meeting the 5mm requirement between the mains and 5V safety requirement.

Why are you using a flip-flop in the same circuit as a microcontroller? Surely the flip-flop can be removed and replaced with a software solution which doesn't take any PCB space.

haxan said:

I want to reduce the size by atleast 30% of the attached circuit.

Click to expand...

Use Photoshop CS5

Why are you using a flip-flop in the same circuit as a microcontroller? Surely the flip-flop can be removed and replaced with a software solution which doesn't take any PCB space.

Click to expand...

Well these microcontrollers are only here to fire TRIAC at specific delays according to 4 bit input coming from another microcontroller which uses BUS architecture. The data from BUS is latched on using the flip flop on this board. I do not think there is any other 4-bit input way other than using serial communication which is a little more complex. The small PIC12 has only 6 I/O pins and 4 are for dimming level (0-100 with a step of 10), 1 for ZC and one is for output pulse which fires the triac.

I would rotate the optoisolators and the graetz bridge so the power line does not pass close to the isolated circuit.

csaba911 said:

I would rotate the optoisolators and the graetz bridge so the power line does not pass close to the isolated circuit.

Click to expand...

Yes, I'd agree, that should also save space.

Best practise is to allocate one section of the PCB for mains and keep everything else at least 5mm away from it. The only things that are allowed to bridge the 5mm no go zone are opto-isolators, Y1 rated capacitors and high voltage resistor and their pads should be at least 5mm either side of the 5mm no go zone.

You're not making full use of the fact that it's a double sided PCB, many connections can be routed via the component side.

Earilier on you talked about using SMT resistors, all I say is be careful with with volage ratings, the 47k resistors need to be able to handel the peak mains votlage and good luck finding SMT resistors that'll do that.

You're lucky this isn't rectified mains (i.e. 325V DC) which requires 7mm clearance because it's the RMS voltage that counts for creepage, not the peak voltage.