PCB design - capacitance between track & ground plane

I read in sci.electronics.design that Daniel Kelly (AKA Jack) wrote (in ) about 'PCB design - capacitance between track & ground plane', on Fri, 23 Jul

2004:

Is this a switch-mode supply? If it is, what is the reactance of 151 pF at the switching frequency? How does that compare with the impedances in your charging circuit?

If not, please look at the following questions:

What is the impedance of 151 pF at DC or 60 Hz? (Hint: infinite and

17.6 gigohms.)

You are applying RF thinking to a very low frequency design. You don't need a ground plane and you can forget about parasitic capacitance.

--
Regards, John Woodgate, OOO - Own Opinions Only. 
The good news is that nothing is compulsory.
The bad news is that everything is prohibited.
http://www.jmwa.demon.co.uk Also see http://www.isce.org.uk

Jack, if the capacitance is of concern, yes, then you can lower the capacitance by not having the tracks on top of each other. If it matters, then you most likely also have to minimize the magnetic field, meaning the tranck should be on top of each other.

I suggest to use heavier Copper, there are manufacturers that do pcbs with 0.3mm, instead of the usual 0.035mm.

And the tracks could become shorter too.

Rene

--
Ing.Buero R.Tschaggelar - http://www.ibrtses.com
& commercial newsgroups - http://www.talkto.net

One would hope so. Parasitics and strays in linear, high-current power supplies! Whatever next?

--

"What is now proved was once only imagin'd." - William Blake, 1793.

Dear John,

Many thanks for your reply.

Yes. It switches at 85kHz.

capacitance.

I want a ground plane for several reasons: (1) to reduce the EMI (2) I need a large ground conductor to deal with the large currents so I might as well use a ground plane, surely?

Thanks, Jack

I read in sci.electronics.design that Daniel Kelly (AKA Jack) wrote (in ) about 'PCB design - capacitance between track & ground plane', on Fri, 23 Jul

2004:

OK, so you should not have looked at the following questions, because they referred to a linear supply.

Not relevant for a switch-mode supply. You should have disregarded it.

Well, that's your choice. There's no clear-cut yes or no for an 85 kHz switching frequency. But 151 pF is 12400 ohms at 85 kHz, so it's not likely to matter. The ground-plane helps with EMC partly *because* of these shunt capacitances.

--
Regards, John Woodgate, OOO - Own Opinions Only. 
The good news is that nothing is compulsory.
The bad news is that everything is prohibited.
http://www.jmwa.demon.co.uk Also see http://www.isce.org.uk

really? you might want to re-think that statement...

have you ever tried using an LM338 (T0-3) without grounding the heatsink - stray capacitance between the device and the heatsink can make them burst into song. Years ago (as an intern) I designed a battery tester tester - a

13.8V 5A power supply that got hit with a pulsed load from the battery-tester under test. And it oscillated. I had built hundreds (literally) of DIY linear psu's before, and never had this problem. I tried all the usual tricks (caps from everywhere to 0V), to no avail. After an entire day of no success, I was almost in tears. My boss (PhD EE and a smart guy) came along, asked what was up so I told him. He looked at my schematic, then the prototype. He picked up a big fat screwdriver, and shorted the heatsink to 0V (the enclosure). It immediately stopped singing.

The problem was twofold: stray C, and a REAL FAST STEP LOAD which excited the oscillatory system. After I grounded the heatsink, I then had to remove all of the stop-it-oscillating caps as my response was very slow. I forget the frequency, but it was fairly fast, many 10s of kHz IIRC.

or build an LDO regulator, which tend to have very high gain, and invariably turn into power oscillators - eg use a NS LP3961 3V3 800mA LDO regulator with 10uF of ceramic output cap - watch it scream! (last-minute change as we couldnt get the spec'd part, and I didnt read the datasheet....doh. nothing replacing the X7R cap with a tant couldnt fix, so the production manager didnt beat me)

cheers Terry

needs to

tracks?

of

a buddy of mine worked for syncor in the late 90's, and he showed me an

8-layer 8-ounce (0.28mm Cu) PCB. It was VERY heavy, and the cross-section looked like almost-solid copper! I used 1-4-4-1 Oz 4-layer boards for a controller/smps for a LED video screen recently.

cheers Terry

Dear John,

Thanks loads for your reply.

So, I guess my last question is: is there any reason why I *shouldn't* remove the ground plane from behind my large top-side conductors? To be honest, I'm not too worried about my circuit producing EMI - but I am keen that it works efficiently.

Many thanks, Jack

Look at the impedance of a battery. A circuit with those kind of current levels won't even notice there's a ground plane there, let alone have to worry about picofarads of strays. IOW, any capacitance to the ground plane would be negligible.

Right. What's the capacitive reactance of that at 120 Hz? What's the equivalent resistance of the battery? What Q does that give you? ;-)

Cheers! Rich

You can use heavier thickness copper like 2oz or 4oz, and you can also tin plate the tracks to make them even lower impedance again. Tight and sensible SMPS circuit layout is what will reduce your EMI the most, a ground plane is not necessarily the answer.

Dave :)

I read in sci.electronics.design that David L. Jones wrote (in ) about 'PCB design - capacitance between track & ground plane', on Mon, 26 Jul 2004:

Tin plating won't have much effect unless it's VERY thick. The resistivity of bulk tin is 7.4 times that of copper, and that of plated tin may well be higher.

--
Regards, John Woodgate, OOO - Own Opinions Only. 
The good news is that nothing is compulsory.
The bad news is that everything is prohibited.
http://www.jmwa.demon.co.uk Also see http://www.isce.org.uk

What is very thick in terms of money? Assuming a thickness of .003" for 2 oz copper and a resistivity of 10 times that of copper for solder then a thickness of .03" would be required to halve the track resistance. Wouldn't it be cheaper to do that, if the solder plating is applied only to the tracks in question, instead of using a 4 oz copper board? Even if my math or theory is off, solder plating seems to be a very sensible alternative to using a thicker copper board since solder paste suitable for tinning is relatively cheap.

I read in sci.electronics.design that Oparr wrote (in ) about 'PCB design - capacitance between track & ground plane', on Mon, 26 Jul 2004:

David L Jones referred to 'tin plating', not 'solder tinning', which can be much thicker than plating, and is what you get using solder paste. 'Solder plating' would not be better than tin plating.

--
Regards, John Woodgate, OOO - Own Opinions Only. 
The good news is that nothing is compulsory.
The bad news is that everything is prohibited.
http://www.jmwa.demon.co.uk Also see http://www.isce.org.uk

If that's exactly what he meant then I'm suggesting that "solder tinning" be used instead. Resistivity isn't the only concern even though obviously addressed, the solder plated track should be able to dissipate more heat even if the track resistance remained the same.

It depends on the type of tin plating, surely you could not be referring to electroless tin plating such as using Tinnit or Cool Amp? Solder plating is

100 times better IMO when it comes to copper tracks.

I was referring to the general "solder tinning" process which you get on typical cheap boards without the solder mask. Although I have seen it many times on boards with solder mask many years ago. That stuff goes on nice and thick and lumpy, thicknesses of 1mm plus are not uncommon. It is an often used method of reducing your track resistance. You can even do it manually by coating your own tracks with solder. This method doesn't look very professional, but it's very effective.

Dave :)

In heard you loud and clear. If you use solder paste and a hot air gun (or a SMD rework hot air tool for better "focus") it can look fairly professional.

tinning" be

to

is