As my design enters the pre-layout stage, I have a number of stupid
newbie questions about PCB.
Hey! You're not a stupid newbie. It takes expirience to be stupid.
Here is my first stupid newbie question. The board that I need to make
is not rectangular, but has an odd shape. (See my previous post about
copying someone else's form factor.) How does one capture the odd shape
(cutouts and shaved corners) in PCB?
Rename one of your drawing layers to be "outline". Draw the outline
on that layer, in 10 mil copper lines.
1. How are odd-shaped boards generally made? Does the PCB manufacturer
make a rectangular board first and then cut/shave/file it down as
necessary?
No, what usually happens is your board is made on a big panel with
other customer's boards. Then, a CNC mill cuts out each board
according to its outline.
You normally have to tell the fab which gerber is your outline, since
they normally have a human looking at it and programming the CNC
router from it.
2. In the .pcb file there is a PCB() or PCB[] record specifying the
board size. Should I set it to the size that the rectangular board
would have had if the answer to Q1 was 'yes', or something different?
(A little larger?)
That's the size of the layout area on the screen. By default, this is
also the size of your board, but if you create an "outline" layer, PCB
uses that instead.
3. In this mailing list traffic I have overheard something called the
outline or fab layer. What exactly is it and how does it work? And
first of all, are "outline layer" and "fab layer" two different terms
for the same thing, or are they two different things?
If you name a layer "outline", PCB treats it different. For example,
it uses it to draw the outline on the "fab" drawing (the fab page in
postscript, or the fab gerber file).
4. What should the outline layer look like? Is it a set of lines and
arcs forming a closed path that encircles the complete shape of the
finished PCB, however odd it is, or just the cutouts? This question
links back to question 2, and is best illustrated by an example.
It should be a series of 10 mil lines and arcs, the *centerline* of
which describes the outline. By "outline" I mean any cut edge,
internal or external. Each FAB has a way of having you tell them
which drawing/file is the outline, often by tagging one of the gerbers
or submitting a README file.
Suppose my finished board needs to look like this:
|<---------------------- 7672 mils ----------------------->|
A| |B
--+-----------------------------------+----------------------+--
^ | | AC mains | ^
| | | connector | | 2040 mils
| | This line is imaginary <--| | |
| | | V
6 | +----------------------+--
5 | |E ^ |F
6 | |<--|-- 2600 mils ---->|
0 | | |
| |
m | | 4
i | | 5
l | | 2
s | | 0 mils
| | |
| | | |
V | | V
--+-----------------------------------+----
C| |D
|<----------- 5072 mils ----------->|
(This is actually a simplification, the real thing is even more complex!)
Here's what my question boils down to: should I make the "total board
size" as reckoned by PCB 7672 x 6560 mils (7672 mils = AB distance, 6560
= AC distance), or something larger?
Either. If you make it larger, you'll be able to, for example, have
elements whose silkscreen goes beyond the edge of the final board.
If I choose the exact ABxAC
dimensions as my PCB size, that'll be the hard boundary of the "world"
within which PCB will allow me to draw on any layer, right? In that
case how would I draw the whole ACDEFB shape on the outline layer?
You can draw *on* the edge of the world boundary, just not *past* it.
Or can one have lines on a layer that run exactly along the edge of
the drawable universe?
Yes.
Or should my outline layer depict just the DEF
cutout (i.e., consist of just two lines: DE and EF), with all other
edges and corners specified implicitly by the "total board size"
setting?
No. An outline layer *replaces* the default outline, it does not
*augment* it.
5. Is the fab/outline layer identified by a special magic layer name in
PCB? Is it "fab" or "outline" or what?
The outline layer is called "outline". The fab drawing is created by
PCB as an output layer, as a combination of the outline layer, a drill
reference, and some other info.
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user