Oops - I accidentally pressed the send button before
ready... So once again:
Plated and non-plated hole of the same diameter need
different drill tools. That is because the plating
process applies copper to the inner wall of the hole,
so you need a thicker drill bit to achieve the correct
diameter.
What your board shop complains about is maybe that
your "drill report file" (*.drr) contains a table
that looks something like
Tool Hole Size Hole Count Plated Tool Travel
---------------------------------------------------------------------------
T1 0.6mm (23.622mil) 193 2112.44 mm (83.17 Inch)
T2 0.8mm (31.496mil) 140 770.14 mm (30.32 Inch)
T3 1mm (39.37mil) 127 1243.70 mm (48.96 Inch)
T4 1.8mm (70.866mil) 34 521.12 mm (20.52 Inch)
T5 3.2mm (125.984mil) 4 538.76 mm (21.21 Inch)
T6 3.25mm (127.953mil) 2 NPTH 269.98 mm (10.63 Inch)
---------------------------------------------------------------------------
Totals 500 5456.14 mm (214.81 Inch)
and your "drill coordinates file" (*.txt) starts with
M71
M48
T1F00S00C0.60
T2F00S00C0.80
T3F00S00C1.00
T4F00S00C1.80
T5F00S00C3.20
T6F00S00C3.25
%
T01
[...]
In this case T6 is marked as non-plated (a mountind hole),
while all other holes are plated, so the board shop has
to override the tool info in the (*.txt)-file with
whatever is appropriate for their process.
This is OK for a double-sided board. But a true single-sided
board cannot have plated throughholes.
What is the bottom line?
Just tell 'em that they should ignore plated/non-plated markers
in your source files.
Cheers
.....
ô ô )
-----oOOo--(_)---oOOo------
Ralf Guetlein
Biotest Medizintechnik GmbH
Industriestrasse 19
D-63755 Alzenau
---------------------------
Tel. +49 6023 9487-42
Fax. +49 6023 9487-35
[EMAIL PROTECTED]
---------------------------
> -----Original Message-----
> From: Thomas [mailto:[EMAIL PROTECTED]]
> Sent: Friday, September 20, 2002 7:39 AM
> To: 'Protel EDA Forum'
> Subject: Re: [PEDA] Unplated pads
>
>
>
>
> > -----Original Message-----
> > From: Rick Wilson (Protta) [mailto:[EMAIL PROTECTED]]
> > Sent: Friday, 20 September 2002 15:06
> > To: 'Protel EDA Forum'
> > Subject: Re: [PEDA] Unplated pads
> >
> >
> > Thomas,
> >
> > Make your bottom layer pads have "NO DRILL" - 0 size -
>
> What??? I'm not sure you understand what I'm on about. How am
> I supposed to
> push the component legs through the PCB without holes?
>
> >I'm sure you don't want to have a bottom layer only pad,
> with a drill?
>
> Yes that's what I want. pads and tracks on one side only and
> unplated holes
> through the pcb.
>
> > It won't work anyway in the manufacturing process.
>
> I don't see why not? I've seen hundreds of single sided pcbs
> like this.
>
> >
> > The other thing I would suggest is to find out why the
> board house is
> > asking for this. Do you supply them with an Excelon Drill
> > file? The .DRL
> > file produced by Protel? If so, they don't need to worry about a pad
> > master.
> >
>
> Actually we supply the .pcb file (allot of ppl in Australia do).
>
> > Last bit of advice. Find another board house.
>
> No. We have a very long standing relationship with this one particular
> company.
> Please keep your advice Protel related.
>
> >
> > Rick Wilson
> >
> >
> >
> > -----Original Message-----
> > From: Thomas [mailto:[EMAIL PROTECTED]]
> > Sent: Thursday, September 19, 2002 7:05 PM
> > To: 'Protel EDA Forum'
> > Subject: Re: [PEDA] Unplated pads
> >
> >
> > The pads are through hole single side only (not SMT).
> >
> > This particular board I'm working on is single sided however
> > it started
> > out as double sided. As things progressed I realised it would
> > all route
> > on a single layer.
> >
> > I can't change the layer stack manager to a single sided
> > board (it seems
> > to think the top layer is being used - but it's not).
> >
> > So I changed all the multilayer pads to bottom layer, hence
> > they had to
> > have their plated attribute turned off.
> >
> >
> >
> > > -----Original Message-----
> > > From: John Haddy [mailto:[EMAIL PROTECTED]]
> > > Sent: Friday, 20 September 2002 11:03
> > > To: Protel EDA Forum
> > > Subject: Re: [PEDA] Unplated pads
> > >
> > >
> > > Are you referring to genuine single sided pads (e.g. surface
> > > mount pads),
> > > or pads with holes that only exist on one side of the board?
> > >
> > > If the former, then I can't imagine why the board shop
> > would make the
> > > request it did, since the pad master would be generated
> > correctly for
> > > the layer required. If the latter, this technology would
> > only be used
> > > for non-plated-through-hole boards, so the existence of imaging
> > > features on
> > > the pad master plot would be irrelevant.
> > >
> > > Personally, I'd go back to the board shop and ask them
> > > specifically why
> > > they've made the request. I HATE having to do workarounds
> > > that have the
> > > potential to support future screw-ups, which is what would
> > happen once
> > > you get into the habit of ignoring all warnings (or turning
> > > them off if
> > > that's possible).
> > >
> > > John Haddy
> > >
> > >
> > > > -----Original Message-----
> > > > From: Thomas [mailto:[EMAIL PROTECTED]]
> > > > Sent: Friday, 20 September 2002 10:34 AM
> > > > To: Protel Data Forum (E-mail)
> > > > Subject: [PEDA] Unplated pads
> > > >
> > > >
> > > > Our board house has asked us to de-check the "Plated" box
> > > for single sided
> > > > pads.
> > > > Ok, 1 global edit later and it's done, only one problem
> > the DRC now
> > > > comes up
> > > > with:
> > > >
> > > > Processing Rule : Broken-Net Constraint ( (On the board ) )
> > > > Violation Net A
> > > > Warning - net contains unplated pads
> > > > Violation Net N/E
> > > > Warning - net contains unplated pads
> > > > Violation Net A1
> > > > Warning - net contains unplated pads
> > > > etc...
> > > >
> > > > I realise these are warnings rather than full blown
> > violations but
> > > > is there any way
> > > > to turn this warning reporting off in the DRC report?
> > > >
> > > > Thanks,
> > > >
> > > > Tom.
> > > >
> > >
> >
>
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
