----- Original Message -----
From: "Brian Guralnick" <[EMAIL PROTECTED]>
To: "Protel EDA Forum" <[EMAIL PROTECTED]>
Sent: Thursday, August 14, 2003 4:57 PM
Subject: Re: [PEDA] PCB Copper thickness VS mounted rails.

> > 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
> be
> > uniform. There is additionally the problem of etching small traces in
> > same layer, due to the thickness.
>     My PCB house says that their process is a positive growth of copper,
> an etch process.  Is this your described "pattern plate"?  When you say
> 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
> and power supply.  3-4 traces are 25 mil wide (audio in), everything else
> at least 50 mil wide, mostly 250 mil wide.

Most boards today have at least one "additive" process, where the outer
layers and all of the drilled holes that are to be "plated thru", get a
layer of electrically plated copper. This usually follows a non electrical
plating process where there is a small amount of "electroless copper"
(copper that is plated / deposited chemically) plates the entire board,
including the inside of the drilled holes, so that the entire board
(including the inside of the holes) can be electrically "charged" so that
electrical plating process will extend into the holes.

Typically, this electrical plating process may plate an equivalent plating
thickness of from 1/2 ounce to 1 ounce of copper, or more.

Thus if you specify 1 ounce of copper for the outer layers of the board,
your board house may start with 1/2 ounce (or less) copper foil on top of
several layers of prepreg, or use a laminate with 1/2 copper (depending on
the stackup), and then "plate up" an additional 1/2 ounce of copper (after
the electroless process), so that the final thickness of copper on the outer
layers is a full 1 ounce, and the copper wall thickness inside the holes is
approximately 1/2 ounce.

This process can vary greatly, depending on just how much copper you specify
on the outer layers and what you want in the wall thickness of the plated
thru holes.

Once the copper is plated up to the final thickness, the board is then
usually masked with the trace pattern and then etched.

There are a few variants to this process.

First, there is the process whereby all of the copper that is to be placed
on the board is added thru selectively plating copper only in the areas
where there is to be copper in the final board. This is an additive process
only, and involves no etching away of any unwanted copper. This process /
method of making boards has been around almost as long (if not longer) as
the etching process, and has been very popular "offshore" where very large
quanties of boards are made and where this process can save lots of money by
not only needing as much (or little) copper as you are actually going to
use, but additionally in the saving of the cost of etchant and echant

Another process, which combines the best of both worlds, is used quite often
by many vendors today. This is the "pattern plating" process (although you
could easily apply this name to the previous process, and this process may
go by different names in some locals). In this process, you begin with a
thin layer of copper on the outer layers (or any other layers for that
matter), of say 1/4 or 1/2 ounce, and then you electrically plate up the
remaining thickness of copper (with or without "electroless" plating as may
be required for plated thru holes). The difference here, is that you first
mask the thin starting layer of copper with an inverse image of the final
copper traces and features, so that you will only plate copper in the areas
that are to have copper in the final design. The next step in this process
would then be to clean off the original mask and then remask only the areas
that you have plated up (which masking can even be done by plating the
conductor pattern with solder, if you use the proper etchant), and then you
etch away the small amount of unwanted copper which remains from the
starting layer of 1/4 or 1/2 ounce copper. Aside from the normal benefits of
using less copper and extending the life of your etchant, there is another
major benefit with this process in that it can yield much better control of
very fine copper features (traces / lines / etc,) since there is much less
copper to be etched (thickness wise), and much less "undercut" in the
etching process. Thus the primary advantage of this process, is the control
of finely etched features. However, there is also a major drawback in using
this process, in that when the entire thin starting layer is masked, and
then when the board is electrically connected to the plating supply (which
makes the whole board become an electrode in the plating process) and
immersed in the plating bath, the amount and distribution of the mask on the
thin starting copper can affect the distribution of the charge of the
surface of the electrode (which is now the board itself), which can cause
different thickness of copper to be plated in different areas of the board.
This type of uneven plating can be controlled to some extent by trying to
distribute the amount of copper that is being used in the design evenly over
the entire surface of the board. Sometimes your board house may add what are
called "robbers" or "thieves" to accomplish this. Some people call this
"balancing" the distribution of copper on a layer, but please note that this
term can easily be confused "balanced copper" or "balancing the copper" in
the design, which is the much older and much more common usage, which refers
to "balancing the copper" placement in the board stackup to prevent board
warpage and delamination.

Back to the problem at hand. Your board shop will probably not start with 4
ounce copper, and then etch thru all 4 ounces. Most likely they will start
with a much thinner starting layer, and then "pattern plate" up to 4 ounces,
or they may even do everything by a totally additive process (I would think
that they are using a normal "pattern plating" process with at least some
etching involved, notwithstanding what they may have told you, and which you
mentioned aboved).

Whether simply plating a full 4 ounces, or pattern plating 2 or 3 or more
ounces, I am sure that there are liable to be several areas on your board
which will present a real challenge to totally even plating resulting in
totally even thicknesses. The thickness being the operative word here in
identifying the problem. The small and minor differences in thickness
encountered in normal pattern plating are going to be magnified several
times in the thickness that you will be using (4 ounces). I would
additionally be concerned with "overhang" in your process, which would be
the opposite of "undercut" in an etching process, but which will surely be
present to some extent in the plating (or "copper growth" as your board
house appears to call it) thicknesses that you are dealing with.

Will it affect your design. The answer is yes, no, and maybe, and it is all
dependant on your board house. The real question is, can they guarantee a
minimum thickness of 4 ounces of copper throughout your entire design,
assuming that you want to use 4 ounces as the number in your current

What is the difference in current carrying capacity for a given width of
trace with a difference in thickness between 3 1/2 ounces of copper and 4
ounces of copper? Are we actually talking about this much difference in the
thickness of copper? It all depends on how good your board house really is,
but I would not rule it out if they are not paying real close attention,
once again, due to the thickness. Remember that 1/2 ounce is 12.5% of 4
ounces, and most board houses only work to +/- 10 % on such things as
thickness and stackup spacings.

Now let me throw in one other variable here, to mess with everybody's mind.
For years I have tried to find out what the difference is in molecular
density between rolled copper sheet (which is very highly compressed due to
the rolling process), and electroplated / electrodeposited copper (which
does not undergo any compression, and which can very due to variables in the
processes involved), such as that which we are talking about in the
manufacture of a pc board. I have talked to many board houses and also many
Chemists about this difference, and they all agree that most likely a there
is in fact a real difference, but no one has been able to point me to a
place to find out just what the difference really is, however, all agree
that a difference in molecular density most probably would directly affect
the current carrying capacity of the specific copper, especially where the
amount of such copper was defined or controlled by its thickness. In other
words, a copper trace, made from 4 ounce rolled sheet, will have a higher
molecular density and therefore carry more current than a trace that
consists entirely or mostly of copper that has been plated up to the same
thickness as the 4 ounce rolled sheet. This actually is an interesting
problem, and I wish that I could find someone who had some real answers to
this issue. The problem in this scenario is that all of the copper used in
the manufacture of printed circuit boards today is defined by thickness, and
only by thickness, notwithstanding the fact that those thickness were
originally derived from the weight of a specific amount of copper rolled to
cover a certain area, and the simple fact is that no one in this industry
ever weighs copper, but simply measures its thickness. When dealing with
only the thicknesses of the copper, the molecular density of the copper
really does make a difference.

Bottom line in your case, if you really are going to use 4 ounce copper, I
would start with rolled copper sheet, especially since you say that there
are no small features that would be affected by the under cut, and design
the widths to account for the large undercut, or at a minimum, start with 2
ounce and plate up the other 2 ounces.

Actually, as mentioned  before (in my last post), I would split the trace
into 2 layers (top and bottom) of 2 ounces each, with a liberal sprinkling
of vias to stitch the 2 traces together.

There is yet one other area where I would think that you might find a
problem in your design, and that is one you have already mentioned in your
previous post, and that is the area of a connection of such parts as a

While I asked in my previous post whether or not your capacitor was large
enough to be available with a "screw mount", so that you could use both
sides of the board as a point of connection, I would additionally think that
it might be helpful in your design to think about soldering a lead on both
sides of the board, if and where you can. While I would still opt for
duplicating the high current traces on both sides of the board, especially
in the area of "mounting pads", with numerous "stitching vias" between them,
this would be an excellent manner of current distribution if you could
access and solder both sides of your connection to the traces on both sides
of the board. (even if you cannot access a joint on the one side of the
board, if you use rosin and the right temperature iron and proper soldering
technique (which I am sure you possess) you can still insure that the solder
'flows" thru the joint to the back side of the board).

Once again I would point out that you would do well to use a much larger
trace than any "current calculator" might recommend, if possible, since you
really don't want to add a "10 degree C rise in temperature" (or more) to
your amplifier, which is where all of the calculators begin their

Anyway, hopefully all of this helpful to you and possibly others who may
read it.


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* 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