[Author Prev][Author Next][Thread Prev][Thread Next][Author Index][Thread Index]
RE: gEDA-user: 2 newbie Qs
Thanks super, D.J. I had visited the gedasymbols.org site, but somehow
managed to consider it just a repository for symbols in the distro. Oops!
What I'm struggling with is a footprint for a LM2575 with a TO-220-5
footprint, which has 5 pins, each pin with max dimensions 0.038 in x
0.025 in, which would lead to a hole dia of sqrt( 0.038^2 + 0.025^2 ) =
0.046 in. Each pin is 0.067 in apart. What I come up with as reasonable
values for thickness, clearance and mask are 0.060 in, 0.014 in and 0.067
in, e.g.
Element[0x00 "TO-220 5 pin" "" "" 10000 10000 0 4800 0 100 ""]
(
Pin[ 0 0 6000 1400 6700 4600 "Pin_1" "1" 0x00000101]
Pin[ 6700 0 6000 1400 6700 4600 "Pin_2" "2" 0x00000001]
Pin[ 13400 0 6000 1400 6700 4600 "Pin_3" "3" 0x00000001]
Pin[ 20100 0 6000 1400 6700 4600 "Pin_4" "4" 0x00000001]
Pin[ 26800 0 6000 1400 6700 4600 "Pin_5" "5" 0x00000001]
)
but looking at it, the solder ring looks really skinny to me. Are those
reasonable values, and am I just an old thick guy? What values would you
use?
And while I'm picking your brain, for a header with 2 mm (0.079 in)
between pins, and pins that are 0.021 x 0.015 in, which I calculate out
as a drill hole of 0.026 (I'll use 0.030 for a little variance,) the
values I'm thinking of using for thickness, clearance and mask are
0.0545 in, 0.049 in and 0.079 in, e.g.
Element[0x00 "2mm header" "" "" 10000 10000 0 4800 0 100 ""]
(
Pin[ 0 0 5450 4900 7900 3000 "Pin_1" "1" 0x00000101]
Pin[ 7900 0 5450 4900 7900 3000 "Pin_2" "2" 0x00000001]
Pin[ 15800 0 5450 4900 7900 3000 "Pin_3" "3" 0x00000001]
Pin[ 23700 0 5450 4900 7900 3000 "Pin_4" "4" 0x00000001]
Pin[ 31600 0 5450 4900 7900 3000 "Pin_5" "5" 0x00000001]
...
What do you think? Reasonable? What would you use?
Many *many* thanks,
Craig
-----Original Message-----
From: geda-user-bounces@xxxxxxxxxxxxxx
[mailto:geda-user-bounces@xxxxxxxxxxxxxx] On Behalf Of DJ Delorie
Sent: Wednesday, September 06, 2006 9:28 AM
To: geda-user@xxxxxxxxxxxxxx
Subject: Re: gEDA-user: 2 newbie Qs
> How do I make a single gschem element that refers to only one of the
> pins, say pin 3?
Create a gschem symbol with one pin. Name it "3".
Go to www.gedasymbols.org and look at Darrell's xilinx symbols.
They're a good example of breaking one footprint up into multiple
symbols.
> 2. In a linear array of pins, say one side of a DIP or a single row
header,
> given a hole diameter H and an interpin distance D (commonly 0.1 inch or 2
> mm, but could be others,) are there any good suggestions for formulas for
> thickness T, mask M and clearance C?
This is subjective. Here's what I do.
For a given line/space (L/S) rule, L+2*S+2 mils between pin copper to
leave room for one trace between pins. If you need two traces, it's
2*L+3*S+2. Thus, for a pin spacing of D, pin copper diameter P is
D-(L+2*S+2) mils.
For small vias, I make the annulus width ((P-H)/2) the same as the
line width (i.e. 20 mil drill = 36 mil copper for 8 mil rules) I'll
use it for (i.e. larger copper for wider traces), up to a maximum
size.
I make mask S/2 mils bigger than the copper, so that the edge is
halfway between the pin copper and the trace copper. For SMD pads
that are too close for a line between, I use G/3 (where G is the gap
between pads) for smaller devices and G/4 for larger ones.
Poly clearance can be anything you want, but it must be at least S. I
used 10 mils in my current project, where lines were 8 mils and the
fab's design rules are 6/6. For SMD parts, I make clearance just big
enough so that there aren't copper strips between pads on small pitch
parts, especially when the strips would be smaller than the design
rules.
Note that fabs often have different rules for inner layers than for
outer layers.
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user
_______________________________________________
geda-user mailing list
geda-user@xxxxxxxxxxxxxx
http://www.seul.org/cgi-bin/mailman/listinfo/geda-user