At 08:43 AM 3/15/01 -0700, Bruce admin wrote:
>I read your email and thought I would throw in my two cents worth. The
>following comments are meant more for educational purposes, and not to
>flame your email. The technology in our field is rapidly changing, and we
>need to help each other keep abreast of these changes. After all, isn't
>that what this forum is all about? Anyhow, read on......
Of course, if we always agreed -- at the outset -- there would be no need
for discussion. Disagreements, if we approach them properly, cause us to
expose the underpinnings of our opinions.
In this case, remember that surface pads were conceived as
surfaces for
>mounting SMT components. Conceptually, they don't have holes, period.
>Probably the dialog box should suppress the hole attribute when the pad is
>assigned to top or bottom. In my opinion, that is the real oversight, that
>such holes are allowed at all.
>
>[Bruce:] This will create problems for people trying to do HDI
>designs. This is the wave of the future with respect to SMD layouts that
>need to be compressed into smaller spaces (better than 50% space savings
>with HDI over conventional SMT designs). Many Japanese designs have been
>using HDI for some time now. I suggest that you read up on this topic to
>gain some insight into where the technology is heading.
Remember, I am *not* talking about the physical structures on the board,
but about how they are represented in a database. *Of course* we need to
have pads with holes. But a "surface pad" is a pad designed for mounting a
surface mount component; and it has a few other innocuous uses as well. But
the structure created for representing a pad with a hole is called a
"Multilayer Pad." It is called multilayer because the hole means that it
has a presence on more than one layer. If there is a hole, it is either a
multilayer pad, or it is a via.
Now, as Bruce quite correctly points out, there are features, particularly
BGAs, which might require a surface mounting pad with a hole in the center.
The database was not designed with these features in mind, so we need to be
careful how we implement them. Because we want solder paste on these pads,
we must use a surface pad (or deal with custom shapes on the paste mask
layer in the footprint, another option). Then we need a hole, typically a
blind via. Protel does not have any entity called a blind pad or which
functions like that except for blind vias. So there is really no choice: a
via must be used for the interlayer hole.
> Otherwise, if a pad has a hole, it is a through hole: i.e., it's
> a hole
>through the board. That's exactly what multilayer pads are, if they have
>holes.
>
>[Bruce:] Not quite true anymore... HDI requires a laser drilled hole,
>often only the first two layers (incredibly small by the way 0.003" to
>0.010"). This is essentially a blind via, but should be defined as part
>of the pad as all interconnects to the surface mount pad will be made
>through these micro vias.
One might like to define such a hole as part of the pad, but that isn't in
the guide book! But one could put blind vias in the footprint. I'm not
certain what the autorouter will do with them, however. If it leaves them
in and routes to them, we are home free. Otherwise, we got trouble in River
City.
> Another issue is raised with this technology though.... It is
> important for some of the emerging technology to have a "window" on the
> surface mount pad for the laser to burn through the outer layers
> (otherwise the laser beam is reflected, etc.). As far as I know, it
> isn't possible yet to define this "copperless window" in Protel yet.
Of course it is possible. In the footprint, place a round feature (I'll get
to that in a moment) at the position of the hole on one of our shiny new
mechanical layers, which will be dedicated to this purpose. We asked for
all those layers so we could do things like this. Then instruct the
photoplotters to merge that layer, as a subtractive negative, with the
normal component side layer. One might be able to make a single file that
would do this with CAMtastic; certainly the RS-274X standard allows for
such. (I've argued for some time that we could get much more efficient
copper pours by using positive/negative merges than by the present draw
method.)
As to the round feature, it could be a pad assigned to the mech layer. Or
it could be an arc of suitable dimensions. Or it could be a very short
piece of track, just long enough that Protel will not think it doesn't
exist. I forget if P99SE deletes zero-length tracks or not. Probably better
to avoid them, because, after all, its undocumented so even if it works, it
might go away in the next rev. Pads on mech layers would be simple and
would not need nets, etc.
> If one wants to put a via in a surface pad, then put a via or
> free pad in a
>surface pad!
>
>[Bruce:] Not really an option for HDI. How difficult do you think it
>would be to make the placement of those HDI micro vias on a fine pitched
>board? I suppose it would work, but personally I would rather define that
>in the decal library.
So put the via in the decal library! The surface pad/hole idea simply would
not work for those blind HDI micro vias.
[...]
{I had written, as an aside:]
>Note that this is not a license for
>via in pad, which can create serious assembly problems!
>
>[Bruce:] Assembly problems are eliminated in HDI (I'm assuming you are
>referring to the solder paste drain problem) because the holes are so
>small that the surface tension will hold the solder on the SMD pad (rather
>than flowing through the micro via). This is well tested and proven in
>Japan (you know how important quality is to the Japanese).
Right. But remember that what is written here will be read by perhaps
thousands of designers of all levels of knowledge and experience. I didn't
want anyone to think that it was okay to put holes in vias without knowing
what you were doing. I've had to fix too many boards with via-in-pad done
by engineers who noticed that they could save a lot of space by putting the
vias in SMT pads. It may work with micro-vias (and I would expect it too,
even more so if the holes are plated shut); it does not necessarily work
with ordinary production-sized vias.
[EMAIL PROTECTED]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To join or leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
