At 07:45 AM 3/11/2002 +0100, Georg Beckmann wrote:

>Make some parts for jumper wire. ( Not any size but a few ).

One might prefer a size appropriate for zero-ohm resistors, which are cheap 
and easier to insert and solder than wires.

If the board is going to be auto-inserted, you will stick with sizes that 
can be auto-inserted.... But if it is manual, you can jump from almost 
anywhere on the board to anywhere else.

To handle connectivity (the rat's nest and DRC), insert your jumpers on the 
schematic as you need them and resynchronize, either with each jumper or 
occasionally. Since the jumpers are parts (even if they are only wires) 
which must be inserted, it is good to have them on the schematic anyway.

>Add teardrops, use not less than pad - hole shoud be not less than 0.8mm.

What is important is not so much hole size as annular ring. On a 
copper-2-side board, the pads on each side plus the plated hole wall plus 
the solder act like a rivet. With a single-sided board, there is only the 
glue underneath the pad to hold the connection to the board; separation of 
this pad (the wires easily break) from the board is a very common cause of 
failure in consumer circuits using single-sided boards.

For this reason, through-hole component leads, if they are at all subject 
to stress, should be clinched so that the lead cannot move even if the 
solder were to melt or crack. Pads should be relatively large; Protel does 
not directly support cut pads (circular pads with the sides cut off, used 
for ICs), other steps should be taken to enlarge pad area. Octagonal pads 
(elongated in one direction) would be great if not for the gerber problems 
due to incorrect Protel implementation. A cut pad can be imitated by 
placing a piece of track on top of a circular pad. The idea is to increase 
pad area while still allowing traces to run between pads.

Preben Lund gives 0.2 mm as the minimum annular ring for non-plated through 
holes. That is pretty small; I'd prefer to see 0.4 mm on a single-sided 
board. I'm used to thinking in mils, and I'd state it slightly smaller: 15 
mils. That means that the pad should be minimum 30 mils over the hole, 
nominal. Holes on single-sided boards are not drilled oversize to allow for 
plating, as they are on double-sided boards, so hole sizes are more 
accurate. One can therefore make the holes a little tighter. Normally, 
holes should be 8 - 20 mils over the size of the lead. For single-sided, 
that could be reduced to 5 mils or so; as long as the lead inserts easily, 
tighter is better. So a 31 mil hole -- a standard drill size -- should be 
fine for IC leads, capacitor, and resistor leads up to 25 mils in diameter. 
This leads to a standard IC pad of 70 mils, with 30 mils in between. That 
isn't enough space to use 20 mil track between pads on 100 mil centers. 
There are a number of possible solutions:

(1) neck the tracks down to 10 mils between pads. Design rule 10/10 
(trace/gap).

(2) neck them down everywhere except for power traces. Design rule 10/10.

(3) reduce pad sizes to 60 mils, preferably with cut pads to beef up the 
pad area. Design rule 20/10, 15/12, or 12/12.

(4) reduce pad size to 50 mils, in which case they *must* be cut pads or 
the like. (Rectangles are not recommended because the sharp corner can help 
start peeling, at least that is the theory). But one could use rectangles 
on the design and then replace the photoplot aperture with a rounded 
rectangle shape.) Design rules 10/10, allowing two traces between pads.

The best path to take depends on the design complexity, process accuracy, 
and production volume.

For bulletproof construction, neck track down only where needed.

>Tracks should be not
>smaller than 0.5mm.

That is too conservative to be an absolute rule, though it would not be bad 
to have such thick tracks (20 mils) except where smaller are needed. In 
fact, I used to use 24 mils routinely for analog design that did not 
require high trace density, necking them down only where needed.

>  Holes should be very thight to the component pins.
>  need lots of different [sizes] also.

Yes to relatively tight holes, but one does not need to be fanatic about 
it. Reducing the number of hole sizes *might* reduce fab cost.

>[..]Are you thinking of a stamped board made from FR2 ?

I've never done a stamped board so I'd be relying on references; my 
comments have been about drilled boards.

>Tell us more about the project.

Always a good idea. The right answers can depend on factors that one might 
easily neglect to include. Are there SMT parts? Is this for a large 
production run? Is it a prototype or lab board, never to be produced in 
large quantities, so saving engineering time may outweigh saving production 
cost. In fact, this could rule out single-sided design, since double-sided 
boards are so cheap and they are stronger.

I've seen single-sided designs produced as double-sided boards. The top 
side was pads only. This might be done for a first-pass prototype for a 
board to be done in large production.

>Every project of this kind I know from ended in a more or less
>big catastrophe.

Single-sided design was pretty routine when I started to design PCBs, and 
my first designs were single-sided copper. I remember doing a single-sided 
parametric equalizer; noise considerations were important, so I couldn't 
just route anywhere I pleased....

But I haven't done a single-sided design for quite a few years. If I were 
designing boards for, say, a consumer product to be made in 100,000 
quantities, saving 50 cents per board, well, do the math. That will pay for 
a lot of engineering time.... But for a single board, saving a few dollars, 
it's not worth it, I wouldn't do it even for hobby use, unless I liked the 
smell of the toxic chemicals and was going to make the board at home.

Abdulrahman Lomax
Easthampton, Massachusetts USA

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to