X-Authentication-Warning: delorie.com: mail set sender to geda-help-bounces using -f
X-Recipient: geda-help AT delorie DOT com
Message-ID: <20191022170155.29708.qmail@stuge.se>
Date: Tue, 22 Oct 2019 17:01:55 +0000
From: "Peter Stuge (peter AT stuge DOT se) [via geda-help AT delorie DOT com]" <geda-help AT delorie DOT com>
To: "John L. Males \(jlmales AT gmail DOT com\) \[via geda-help AT delorie DOT com\]" <geda-help AT delorie DOT com>
Subject: Re: [geda-help] Question: New User - How To Create Very Simple
 Unique PCB With No Components
References: <20191019020002 DOT 088a8f4fa249e251d11adfe5 AT gmail DOT com>
 <CAHUm0tM+R8PORa+US2Nt0Q1vaU80YcG9AEyH8XWUVODJAV09aA AT mail DOT gmail DOT com>
 <CAJZxidBbky8CT7mcRa1DX_pZTLnf=x2x0Hh4CiX122F-F_c1Vw AT mail DOT gmail DOT com>
 <20191020183718 DOT e6fccd7def16f88626a4fa24 AT gmail DOT com>
 <CAHUm0tM-w4Y-AazjhGX4wC8R1Pq1Cgr0S6AZ3O+5LFGHUixkAg AT mail DOT gmail DOT com>
 <20191021024423 DOT 8d189fc5ca003a8a11384366 AT gmail DOT com>
 <CAHUm0tNgLr71gWeMeGKQD9ZEtOo-nPYmcOxT4GZ7TTBV36Z8NQ AT mail DOT gmail DOT com>
 <20191021213833 DOT 6bef6a8bfbaf6d69e36c2527 AT gmail DOT com>
 <CAJZxidAL_hu6Kjs6G09xBaBS6ibvxP1+tGAHnOqA2A=HRdnkGQ AT mail DOT gmail DOT com>
 <20191022024127 DOT bb67cfef6635bc82b8c747a4 AT gmail DOT com>
MIME-Version: 1.0
Content-Type: text/plain; charset=utf-8
Content-Disposition: inline
Content-Transfer-Encoding: 8bit
In-Reply-To: <20191022024127.bb67cfef6635bc82b8c747a4@gmail.com>
Reply-To: geda-help AT delorie DOT com
Errors-To: nobody AT delorie DOT com
X-Mailing-List: geda-help AT delorie DOT com
X-Unsubscribes-To: listserv AT delorie DOT com
Precedence: bulk

John L. Males (jlmales AT gmail DOT com) [via geda-help AT delorie DOT com] wrote:
> Is the "Pin" attribute of the part "Element" a Via or just a
> pin with hole for the layer the pin is assigned to?

A Pin inside an Element is on one hand a connection point for one part
in the netlist (irrelevant for your board) and on another hand a
drilled hole through all layers and a copper ring on all layers.

This is far more than you need. By adding the "hole" flag to the Pin
you can indicate that this Pin is actually primarily a hole. Here's a
footprint that I've created for a single M3 mounting hole:

Element[0x00000000 "M3 mount" "" "" 0 0 -1mm -1mm 0 100 ""]
(
        Pin[0 0 3.6mm 0.4mm 3.4mm 3.2mm "" "1" "hole"]
)

3.2mm is the drill diameter. What are the 3.6, 0.4 and 3.4 measurements?

3.6mm is Thickness - the outer diameter of the copper ring, were this
Pin not a hole. Being a hole, no copper ring is generated.

0.4mm is Clearance - add this to Thickness above to get the diameter of
the generated copper removal around the center of the hole. This applies
equally to holes (with "hole" flag; no copper) and pins (without "hole"
flag).

3.4mm is Mask - diameter of the generated circular opening of the
solder mask around the center of the hole. Applies to holes and pins.


> For example I have created a part that is just the set of holes using
> the "Pin" attribute of the part "Element" so the set of 6x3 holes is
> spaced exactly as needed and with a home reference point.

That's a great solution.


Some general points:

I've not seen any PCB fab offer 3-layer boards. You can get 1, 2 or 4.
You'll do fine with 2.

Please mind that PCB thickness is very much inexact. Fiberglass cores
(sometimes called prepreg) are built by the PCB fab stacking multiple
10-100µm layers to roughly the required height. This is a mechanical
process which has variations - those may be quite significant,
depending on which capacitance tolerance you require. Expect no less
than ±100µm thickness tolerance.

Please also do research different dielectric materials. FR4 is the
entry level material, quite a loose weave, exhibiting fairly high
variation. Many PCBs with strict signal integrity requirements can
not afford to use FR4, but need a much tighter weave in the core,
to reduce dielectric constant variation significantly. You may or
may not need to consider this, and may have to work with select,
higher-end PCB fabs who control more precise processes and offer
different core materials, again depending on your tolerance requirement.

Remember to leave any area of the PCB which rests against metal
(on the back if I understood you correctly) free of copper, even
if you use solder mask. The solder mask is a think lacquer and will
wear off with friction.

And remember to leave at least 0.5mm to the PCB edge free of copper.


In North America you could start with ordering PCBs from oshpark.com,
they do efficient pooling such that you don't have to pay much per
board. If you have the time this means you can do a test run or two
of just a few boards, on one hand to practice the process with your
software before contacting a higher-end fab, on another hand to get
some actual boards to test functionally.



Kind regards

//Peter