Hello Matthew and Kitty,
It's not too often that you can answer two queries with one post, but
both of your posts are closely related.
AFIK, the problem is not so much with etching, but with plating density.
That is the electro-plating of copper following the electro-less copper
process. The board's unmasked copper pattern becomes part of an electric
circuit in the electro-plating process. Which is all fine if the pattern
is an even distribution of copper over the entire board.
However, if there is a heavy copper area at one corner of the board and
fine tracks at the other, then the current flow in the plating process
will favour the path of least resistance - the heavy copper area. So,
you get uneven copper thickness across the board. The thin tracks at the
bare end of the board end up with less copper before the etching process
(which is fairly even with spray etchers).
One technique to help this is to use hatching in the heavy copper area
to reduce the surface area of the copper compared to a solid fill.
Another is to add thieving to the bare areas to increase the surface
area of the copper in those areas.
I believe that you are right to avoid having an excessive imbalance of
copper on one side of the board as well.
Shielding wise, the hatching will work depending on your hatching
spacing compared to the wavelength of frequencies of interest (Faraday
shield). Only other concern is for current carrying capabilities.
In earlier days, I believe that hatching was preferred to avoid large
areas of meltable (solder plating) metals under the solder mask. This
would cause the mask to wrinkle under reflow. (That was when the solder
plating was used as an etch resist - this is no longer the case.)
Another reason to leave a lot of copper on the board is to reduce the
amount that has to be etched off and disposed of.
The question of using hatching in preference to solid fill depends on
how dense the rest of your board is.
On the subject of thieving patterns, our EMC expert here generally
advises to have small areas of unconnected copper if really needed. Many
fab housed can add this in their CAM if you allow them and provide
spacing guidelines etc on your master drawing. If your copper pour is
functional eg. 0V then EMC may even improve. You have to be careful in
the application of additional pours and theives in video / RF /
controlled impedance / ethernet areas. In this application they can
affect the operation of the circuit due to many effects, particularly
capacitive coupling, so are not advised here.
regards,
Phil.
-----Original Messages-----
From: Matthew Lamkin [mailto:[log in to unmask]]
Sent: Monday, 12 August 2002 21:09
To: [log in to unmask]
Subject: [DC] Copper areas, To hatch or not to hatch?
Hello, I am having a small discussion with one of the engineers at the
moment about groundplane
and whether or not it should be hatched or solid?
AFAIKR if you have large areas of copper on a board with lots of thin
tracks
it can cause etching problems because the
board is not even, so some of the thinner tracks can get etched away.
Also, when it is sent through the hot processes (Reflow/wave etc) it can
cause the board to warp, if one side has more large areas
of copper on than the other.
Hatched copper is supposed to prevent both these from happening.
For a small digital board that does not have high currents going through
it
solid groundplane is not required and hatched will suffice.
I have seen many modern PC cards that use hatched grounding on.
Now the big question is "am I talking codswallop here" or what?
I'd appreciate some comments from you more experienced engineers.
P.S. I'm referring to single/double sided boards only not Multilayer.
(although I'd appreciate comments regarding those as well to cope with
my
current 4L board).
Thankyou,
Matthew Lamkin.
And, closely related....
Hi,
I've been advised by the board house to add copper thieving to the outer
layers of a design we've sent them for manufacturing. I understand they
need to add copper in bare areas to allow them to plate evenly across
the board. We're considering a copper pour as opposed to sporatic field
oof copper squares...any suggestions, advice, comments?
Thanks for your input,
Kitty
------------------------------------------------------------------------
---------
DesignerCouncil Mail List provided as a free service by IPC using
LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text
in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To set a vacation stop for delivery of DesignerCouncil send: SET
DesignerCouncil NOMAIL
Search previous postings at: www.ipc.org > On-Line Resources & Databases
> E-mail Archives
Please visit IPC web site http://www.ipc.org/html/forum.htm for
additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700
ext.5315
------------------------------------------------------------------------
---------
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To set a vacation stop for delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/html/forum.htm for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-509-9700 ext.5315
---------------------------------------------------------------------------------
|
