[Fwd: Re: [sdiy] JH goes PCB - Copper ring size for PCBs?]

[Seb Francis]

Meant for list I think...

-------- Original Message --------
Subject: 	Re: [sdiy] JH goes PCB - Copper ring size for PCBs?
Date: 	Thu, 17 May 2007 10:35:13 -0400
From: 	Tom Corbitt <tom.corbitt at gmail.com>
To: 	Seb Francis <seb at burnit.co.uk>
References: 	<003601c79871$425a9eb0$0300a8c0 at jhsilent> 
<464C448D.3050800 at burnit.co.uk>



Most of the shops I've dealt with over the years require a min annular 
ring of 5mils (0.127mm). It's possible to go smaller, but there is 
usually extra $$ involved. The reason is that the larger the ring, the 
looser the fab house can be with their drill hits. Under 5mils or so and 
it's very likely that any drill hit will be off center enough to 
comprise the pad/via edge which can lead to mechanical issues.

The formula is (Outer-Inner)/2. For example a via with an outer diameter 
of 28mils and a inner hole of 18mils would pass the 5mils rule (I just 
always make sure that my outer is at least 10mils (0.254mm) larger then 
the inner hole.

I also try to stay away from the fixed drill size houses unless I design 
for them up front as what you get can be very different from what you 
asked for.

tom c.

On 5/17/07, *Seb Francis* <seb at burnit.co.uk <mailto:seb at burnit.co.uk>> 
wrote:

    A couple of things:

    Normally manufacturers assume the size you specify is the finished hole
    size, not the actual drill size.  So you shouldn't need to think about
    the thickness of the plating through the hole, only about what size
    component legs you want to push through the finished hole.

    However just be confusing, the manufacturers I know spec the minimum
    annular ring width with regard to the Production Hole Diameter (the
    drill size itself).  The actual minimum annular ring width will vary
    from manufacturer to manufacturer, but a typical value is 0.15mm.  Thus
    your pad diameter must be 0.3mm larger than the Production Hole Diameter
    (drill size), or 0.4mm larger than the finished hole size.

    So Hole = 0.9mm, Pad = 1.5mm sounds easily ok (but do check the minimum
    annular ring specs of your manufacturer)

    Seb


    JH. wrote:
     > I'm editing some library elements of my Rimu PCB layout tool for
    the use
     > with Olimex:
     >
     > Olimex web site says that final hole diameter will be 0.1mm
    smaller than
     > drilled because of plating of the holes, and consequently offer
    "odd" drill
     > diameters as a standard, like 0.9mm and 0.7mm, to get the
    "standard" holes
     > of 0.8mm and 0.9mm.
     >
     > So, ist it ok to increase the hole size in the library without also
     > increasing the pad diameter?
     > Specifically, is the combiantion
     >
     > Hole = 0.9mm, Pad = 1.5mm ok ?
     >
     > (Talking of double sided boards - I know it's probably not large
    enough for
     > single sided ...)
     >
     >
     > Hmmm, yes ... I think I'm going to make pcbs again after many
    years of
     > Veroboard-only.
     > And I hope it will be for the benefit of the DIY comunity, too! :)
     >
     > And I just found that I *might* get the whole lot of filterbanks and
     > envelope detectors of a Sennheiser vocoder
     > on a single 320 x 200 mm board, when I completely redesign the
    circuit
     > topology ...
     >
     > JH.
     >
     > _______________________________________________
     > Synth-diy mailing list
     > Synth-diy at dropmix.xs4all.nl <mailto:Synth-diy at dropmix.xs4all.nl>
     > http://dropmix.xs4all.nl/mailman/listinfo/synth-diy
     >
     >

    _______________________________________________
    Synth-diy mailing list
    Synth-diy at dropmix.xs4all.nl <mailto:Synth-diy at dropmix.xs4all.nl>
    http://dropmix.xs4all.nl/mailman/listinfo/synth-diy