PCB design - capacitance between track & ground plane

[Daniel Kelly \(AKA Jack\)]

Hi,

I'm designing a PCB for a high-current battery charger. My charger needs to
deliver in excess of 10 amps.

This current requires big, fat tracks.

But I'm worried that big fat tracks will also have a fat parasitic
capacitance (I'm using double sided board with the bottom layer being my
ground plane).

So, my question is: should I remove the ground plane under my fat tracks?

My calculations suggest that my fattest track would have a capacitance of
151pF.

Links:

Images of my draft schematic and board designs:
http://www.ucl.ac.uk/~ucgadak/board.gif
http://www.ucl.ac.uk/~ucgadak/schematic.gif
(this design uses components that will only deliver 4 amps, but I want the
PCB to be 'upgradeable' to 10 amps)

Datasheet for the chip I'm using:
http://www.maxim-ic.com/quick_view2.cfm/qv_pk/3483

Maths for capacitance:
http://www.informit.com/articles/article.asp?p=169477&seqNum=6

Many thanks,
Jack

 

[John Woodgate]

I read in sci.electronics.design that Daniel Kelly (AKA Jack) <d.kellyNO
[email protected]> wrote (in <[email protected]>) about
'PCB design - capacitance between track & ground plane', on Fri, 23 Jul
2004:

I'm designing a PCB for a high-current battery charger. My charger
needs to deliver in excess of 10 amps.

This current requires big, fat tracks.

But I'm worried that big fat tracks will also have a fat parasitic
capacitance (I'm using double sided board with the bottom layer being my
ground plane).

So, my question is: should I remove the ground plane under my fat
tracks?

My calculations suggest that my fattest track would have a capacitance
of 151pF.

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.

 

[Rene Tschaggelar]

Hi,

I'm designing a PCB for a high-current battery charger. My charger needs to
deliver in excess of 10 amps.

This current requires big, fat tracks.

But I'm worried that big fat tracks will also have a fat parasitic
capacitance (I'm using double sided board with the bottom layer being my
ground plane).

So, my question is: should I remove the ground plane under my fat tracks?

My calculations suggest that my fattest track would have a capacitance of
151pF.

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

 

[Paul Burridge]

I read in sci.electronics.design that Daniel Kelly (AKA Jack) <d.kellyNO
[email protected]> wrote (in <[email protected]>) about
'PCB design - capacitance between track & ground plane', on Fri, 23 Jul
2004:

Is this a switch-mode supply?

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

 

[Daniel Kelly \(AKA Jack\)]

Dear John,

Many thanks for your reply.

Is this a switch-mode supply?

Yes. It switches at 85kHz.

You don't need a ground plane and you can forget about parasitic

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

 

[John Woodgate]

I read in sci.electronics.design that Daniel Kelly (AKA Jack) <d.kellyNO
[email protected]> wrote (in <[email protected]>) about
'PCB design - capacitance between track & ground plane', on Fri, 23 Jul
2004:

Many thanks for your reply.


Yes. It switches at 85kHz.

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

capacitance.

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

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?

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.

 

[Terry Given]

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

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

 

[Terry Given]

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

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

 

[Daniel Kelly \(AKA Jack\)]

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

 

[Rich Grise]

Hi,

I'm designing a PCB for a high-current battery charger. My charger needs
to deliver in excess of 10 amps.

This current requires big, fat tracks.

But I'm worried that big fat tracks will also have a fat parasitic
capacitance (I'm using double sided board with the bottom layer being my
ground plane).

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.

So, my question is: should I remove the ground plane under my fat tracks?

My calculations suggest that my fattest track would have a capacitance of
151pF.

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

 

[David L. Jones]

Hi,

I'm designing a PCB for a high-current battery charger. My charger needs to
deliver in excess of 10 amps.

This current requires big, fat tracks.

But I'm worried that big fat tracks will also have a fat parasitic
capacitance (I'm using double sided board with the bottom layer being my
ground plane).

So, my question is: should I remove the ground plane under my fat tracks?

My calculations suggest that my fattest track would have a capacitance of
151pF.

Links:

Images of my draft schematic and board designs:
http://www.ucl.ac.uk/~ucgadak/board.gif
http://www.ucl.ac.uk/~ucgadak/schematic.gif
(this design uses components that will only deliver 4 amps, but I want the
PCB to be 'upgradeable' to 10 amps)

Datasheet for the chip I'm using:
http://www.maxim-ic.com/quick_view2.cfm/qv_pk/3483

Maths for capacitance:
http://www.informit.com/articles/article.asp?p=169477&seqNum=6

Many thanks,
Jack

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

 

[John Woodgate]

I read in sci.electronics.design that David L. Jones
gle.com>) about 'PCB design - capacitance between track & ground plane',

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.

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.

 

[Oparr]

Tin plating won't have much effect unless it's VERY thick.

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.

 

[John Woodgate]

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.

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.

 

[Oparr]

David L Jones referred to 'tin plating', not 'solder tinning'

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.

 

[David L. Jones]

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

 

[Oparr]

I was referring to the general "solder tinning"

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.

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 [/QUOTE]