X-Authentication-Warning:	delorie.com: mail set sender to geda-user-bounces using -f
X-Recipient:	geda-user AT delorie DOT com
Date:	Wed, 25 Jul 2012 14:34:18 -0700
From:	Colin D Bennett <colin AT gibibit DOT com>
To:	geda-user AT delorie DOT com
Subject:	Re: [geda-user] how to use "clearance" and mask in pcb footprint
Message-ID:	<20120725143418.5f735b1d@svelte>
In-Reply-To:	<5010D52B.8030800@plastitar.com>
References:	<CA+GuLwe5sPPWJQAQtX2mYTFYz5Dnt_wPy42ywZnY37dagsrEHQ AT mail DOT gmail DOT com>
	<5010D52B DOT 8030800 AT plastitar DOT com>
X-Mailer:	Claws Mail 3.8.0 (GTK+ 2.24.10; x86_64-pc-linux-gnu)
Mime-Version:	1.0
X-AntiAbuse:	This header was added to track abuse, please include it with any abuse report
X-AntiAbuse:	Primary Hostname - gator297.hostgator.com
X-AntiAbuse:	Original Domain - delorie.com
X-AntiAbuse:	Originator/Caller UID/GID - [47 12] / [47 12]
X-AntiAbuse:	Sender Address Domain - gibibit.com
X-BWhitelist:	no
X-Source:
X-Source-Args:
X-Source-Dir:
X-Source-Sender:	(svelte) [65.61.115.34]:33278
X-Source-Auth:	colin AT gibibit DOT com
X-Email-Count:	2
X-Source-Cap:	c2t5bGVuO3NreWxlbjtnYXRvcjI5Ny5ob3N0Z2F0b3IuY29t
Reply-To:	geda-user AT delorie DOT com
Errors-To:	nobody AT delorie DOT com
X-Mailing-List:	geda-user AT delorie DOT com
X-Unsubscribes-To:	listserv AT delorie DOT com

On Thu, 26 Jul 2012 01:27:07 -0400
Phil Taylor <phil AT plastitar DOT com> wrote:

> On 7/25/2012 12:05 PM, Ram Bhamidipaty wrote:
> > I'm pretty sure the way I am doing the pins with the mask and
> > clearance values is wrong. Are there some general rules I
> > should follow for solder mask and clearance values? Are
> > clearance and mask values dependent on the board fab rules?
> 
> Ram,
> 
> This document explains the clearance and mask numbers ... which
> are not as obvious as you might at first think.
> 
> The design rules in PCB do not modify file footprints.  The
> footprints are what they are ... when you write them.  This would
> pertain to text-written file type footprints.  I have no idea
> about footprints created in PCB's gui.

The design rules in pcb aren't related to footprint clearance and
mask settings, except that if the clearance to polygons is too
small, it could violate design rules of a specific layout and cause
a DRC error.

Footprints created in pcb's GUI by drawing them will save
mask/clearance settings based on the route style selected (e.g.,
Signal, Power, Fat, ...) unless you modify these mask/clearance
settings first manually.

The weird thing about mask and clearance is how they are specified:

    # Clearance: add to thickness to get clearance diameter
    # Mask: diameter of solder mask opening

This means for example if you have a 20 mil wide pad (think of it
as a LINE, since that's what it is), and you want 12 mil clearance
to polygons with 3 mil gap from solder mask to copper, set the
following **in the .fp footprint file** (not using pcb GUI, since
it uses a different scheme!!)

 thickness = 20mil               # Note: copper "diameter"
 clearance = 2 * 12mil = 24mil   # Note: just the diameter increment
 mask      = 20mil + (2 * 3mil) = 26mil   # Note: total diameter

Like this:

Element["" "" "" "" 1430.00mil 1860.00mil 0.0000 0.0000 0 44 ""]
(
    # ------------------------------------------------------------------
    # Pad[    rX1    rY1     rX2     rY2  Thickn   Clr      Msk     Nm  Nr  Fl]
    # ------------------------------------------------------------------

    Pad[-110.00mil 0.0000 60.00mil 0.0000 20.00mil 24.00mil 26.00mil "1" "1" ""]
    # Pad 20 mil wide
    # Clearance to polygons: gap = 12 mil ( = 24mil/2)
    # Gap to solder mask: 3 mil = (26mil-20mil)/2
)

It's a cumbersome and annoying, but you just have to get used to
it. The problem is that we usually want to specify footprint specs
in different terms than pcb requires them, like we want to say "gap
from copper to solder mask" or "gap between pad and polygon".  It
would be so nice to have cleanly described footprints, rather than
relying on layers of footprint generator scripts and stuff, or
tedious manual calculations.

Regards,
Colin

- Raw text -