> The problem with calling out 4 oz. Cu, or even 2 oz. for that matter, is
> that the board house will probably "pattern plate" the Cu, and it may not
be
> uniform. There is additionally the problem of etching small traces in the
> same layer, due to the thickness.

    My PCB house says that their process is a positive growth of copper, not
an etch process.  Is this your described "pattern plate"?  When you say "not
uniform", how much error can I expect?  Will it matter with traces from 50
mil to 500 mil.

   My PCB does not have any fine traces.  It's a pure CMOS class A audio amp
and power supply.  3-4 traces are 25 mil wide (audio in), everything else is
at least 50 mil wide, mostly 250 mil wide.

_____________
Brian Guralnick
[EMAIL PROTECTED]


----- Original Message ----- 
From: "JaMi Smith" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Cc: "JaMi Smith" <[EMAIL PROTECTED]>
Sent: Thursday, August 14, 2003 2:44 PM
Subject: Re: [PEDA] PCB Copper thickness VS mounted rails.


> Brian,
>
> Sorry for the late response, but here goes.
>
> The problem with calling out 4 oz. Cu, or even 2 oz. for that matter, is
> that the board house will probably "pattern plate" the Cu, and it may not
be
> uniform. There is additionally the problem of etching small traces in the
> same layer, due to the thickness.
>
> Solder, or solder plate (with or without soldermask so that you can put
more
> on), as brought out in an earlier post, is a very very poor design choice,
> simply because solder will only carry about 16 percent of the current that
> copper will. You should never rely on solder to carry any current
> whatsoever. This is why solder is always excluded in any current carrying
> capacity calculations, whether they be the old MIL STD 275 calculations or
> charts, or any of the numerous newer ones (the IPC charts are the same as
> the old 275 charts).
>
> Bus bars do offer a solution, as does plain old wire.
>
> I would opt for the wider traces, as brought out in one earlier post, and
I
> would distribute the copper on both sides of the board, and stitch it
> together with a very liberal sprinkling of vias, which should allay your
> fears about the connections that you bring up below. Remember to account
for
> the size of the vias in your trace width calculations (subtract out the
hole
> size(s) from the width of the trace)).
>
> Is it possible that the caps are large enough to have screw type
terminals?
> If so, you could possibly use a wire with a terminal, in addition to the
> copper traces.
>
> Someone also mentioned a 10 - 15 degree C rise in conductor temperature in
> an earlier post. That is one problem with most "current capacity
> calculators" today, is that they start at 10 degrees C, and the fact is
that
> you really do not want to design in a 10 degree C rise in temperature to
> your product, not to mention 15 degrees C or anything higher. In reality,
> unless you have a lot of airflow and lots of extra cooling capacity, you
> really should be designing for something mush less than 10 degrees C for
the
> normal operation of the product. If you get large surges in current that
> last for any considerable length of time, and you get them often, then
maybe
> it is time to increase your nominal / normal current rating a bit.
>
> JaMi
>
> ----- Original Message -----
> From: "Brian Guralnick" <[EMAIL PROTECTED]>
> To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Sent: Friday, August 08, 2003 10:26 AM
> Subject: Re: [PEDA] PCB Copper thickness VS mounted rails.
>
>
> > > One other possibility is to make the board double sided, with 3 Oz
foil
> > > on each side.  This will be easier for them to etch/plate, and
> > > paralleling the
> > > high current traces on two layers gives the same resistance.  I guess
> this
> > > won't work if this is a thermal board to be bonded to a heat sink.
> > >
> > > Jon
> >
> >     I don't like making power supply PCBs with power traces on both
sides.
> > Especially with large snap-in caps.  It is too difficult to ensure that
> the
> > top of the PCB under the cap has a good solder to the huge fat traces
just
> > like the bottom.  I've experienced such designs where power supply
> sections
> > get a fine odd crackling type noise, which may be mistaken for a bad
caps,
> > but it really was fine cracks in the solder on the top layer just under
> the
> > cap.  With a 1 layer board, such a problem is easily caught.
> >
> >
> > _____________
> > Brian Guralnick
> > [EMAIL PROTECTED]
> >
> >
> > ----- Original Message -----
> > From: "Jon Elson" <[EMAIL PROTECTED]>
> > To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> > Sent: Monday, August 04, 2003 1:59 PM
> > Subject: Re: [PEDA] PCB Copper thickness VS mounted rails.
> >
> >
> > >
> > >
> > > Brian Guralnick wrote:
> > >
> > > >I'm designing a power supply with will have a large ripple current.
> This
> > > >power supply will be on it's own PCB and it's 1 layer.  Am I better
off
> > > >mounting high current rails, or, increasing the PCB copper thickness
> from
> > > >1oz to something like 4-6oz?
> > > >
> > > >The power supply will be 90 vdc, continuous dc current of 4 amps,
with
> > > >current surges & ripple current above 15 amps.
> > > >
> > >
> > > >Check with your PCB vendor on how much the extra thickness of copper
> > > >
> > > will cost you.  Then, compare with the rails, including the cost of
> having
> > > the assemblers deal with it.  If the 4 or 6 Oz foil will carry the
> > > current with
> > > acceptable electrical characteristics, it sounds like the best
solution,
> > > unless
> > > the extra cost is prohibitive.  My guess is the extra foil thickness
> will
> > be
> > > cheaper than all the extra handling to assemble the whole thing.
> > >
> > > One other possibility is to make the board double sided, with 3 Oz
foil
> > > on each side.  This will be easier for them to etch/plate, and
> > > paralleling the
> > > high current traces on two layers gives the same resistance.  I guess
> this
> > > won't work if this is a thermal board to be bonded to a heat sink.
> > >
> > > Jon
> > >
> > > >
> > > >
> > >
> > >
> > >
> >
> >
>
>



* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to