Connect with us

PCB design - capacitance between track & ground plane

Discussion in 'Misc Electronics' started by Daniel Kelly \(AKA Jack\), Jul 23, 2004.

Scroll to continue with content
  1. 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
     
  2. I read in sci.electronics.design that Daniel Kelly (AKA Jack) <d.kellyNO
    > wrote (in <cdqmi7$2ldc$>) 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.
     
  3. 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
     
  4. One would hope so. Parasitics and strays in linear, high-current power
    supplies! Whatever next?
     
  5. 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
     
  6. I read in sci.electronics.design that Daniel Kelly (AKA Jack) <d.kellyNO
    > wrote (in <cdrqjd$313s$>) 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.
     
  7. Terry Given

    Terry Given Guest

    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
     
  8. Terry Given

    Terry Given Guest

    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
     
  9. 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
     
  10. Rich Grise

    Rich Grise Guest

    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
     
  11. 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 :)
     
  12. I read in sci.electronics.design that David L. Jones
    gle.com>) about 'PCB design - capacitance between track & ground plane',
    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.
     
  13. Oparr

    Oparr Guest

    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.
     
  14. 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.
     
  15. Oparr

    Oparr Guest

    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.
     
  16. 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 :)
     
  17. Oparr

    Oparr Guest

    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.

    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]
     
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-