Thanks Ralf, that makes sense. I sort of suspected that was their reasoning.

I suppose the way around this is to leave the pads attributes as "plated"
but tell the board shop to ignore it.

But...

What about a board with mixed plated and unplated holes (perhaps for
clearance reasons on the top layer, a through hole multilayer pad was made
unplated bottom side only)?

Is it possible to tell Protel to ignore the warnings of *possible*
unconnected nets due to unplated pads in this case?

It seems that Protel can't tell if there is a track connected to a pad that
was multilayer but then changed to single side unplated.

i.e. when a through hole multilayer pad is changed to top side unplated,
Protel DRC should do:

top unplated pad to top track (same net) = ok

bottom track to top unplated pad hole location (or anywhere else
unconnected) = unconnected net violation

Instead the DRC gives an unconnected net warning for *every* unplated pad
even if the net is unbroken due to the track and single sided pad being on
the same layer. 

The ratsnest connection layer can sort it out, why can't the DRC?

Is this a problem with converting multilayer pads to single side unplated?
or
Is it just damn lazy programming?
or
Am I missing something? It is Friday and I've had a few knock off beers.

Have a good weekend all.

Tom.



> -----Original Message-----
> From: "GŁtlein, Ralf" [mailto:[EMAIL PROTECTED]]
> Sent: Friday, 20 September 2002 17:39
> To: Protel EDA Forum
> Subject: Re: [PEDA] Unplated pads
> 
> 
> 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
> 
>            .....
>            Ű Ű )
> -----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
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to