gEDA-user: Re: soliciting suggestions on making drill/fabrication drawings from Excellon drill files, or another PCB manufacturer

[Ales Hvezda <ahvezda@seul.org>]

[ Ales here, I'm reposting this since majordomo didn't recognize the
  e-mail as being subscribed to the geda-dev mailinglist. ]

-- Cut here --
From: harry eaton <haceaton@aplcomm.jhuapl.edu>

Charles Lepple wrote:

> I'm beginning to wonder if anyone out there uses pcb-1.6.3 or its 
> successors for actual prototypes anymore :-(
>
> I have a board design drawn with pcb-1.6.3, and I want to get it 
> manufactured. The folks at work have had almost nothing but good 
> things to say about Advanced Circuits (http://www.4pcb.com), so I'm 
> working with them right now. 

I have made a few boards through Advanced Circuits, and they seem to 
always have problems, even when the files load perfectly with Gerbtool, 
which is what they use for manufacturing. I've always been able to get 
them to eventually fab the board (correctly), after telling them a few 
times "it looks perfect to me when I view it with Gerbtool". Often a 
"supervisor" has to solve a computer-crashing type problem.

>
>
> Problem is that PCB doesn't generate a fabrication or drawing (just 
> the Excellon drill programming file). I figured I might be able to 
> stitch together a bunch of the PostScript output files and edit in 
> some drill identifiers, but that didn't work. 

I'll have to look at the "drill helper" output with postscript, but I 
thought this was more-or-less an un-dimensioned fabrication drawing as 
far as drilling was concerned.

>
>
> From what I gather, they want a drawing that shows different markings 
> at each drill hit. It seems like more of a sanity check than an 
> absolute manufacturing requirement, but apparently if you get the 
> $33/each special from this place, you don't get the full PCB file 
> fixing service. 

Ah yes, well I've never tried their $33 service. Olimex is good for that 
though and they never complain.

>
>
> I wouldn't be so concerned about the drill program (after all, it 
> works fine in gerbv) but Lavenier's (sp?) ViewMate program misaligns 
> the drill and Gerber files, and so does freedfm.com (4pcb.com's online 
> design-for-manufacturability checker).
>
> I'm not sure what I need, really. If anyone has a favorite PCB fab 
> that can handle pcb's Gerber and drill files right off the bat, I'll 
> consider it. Or, pointers to Excellon drill-to-drawing (PostScript, or 
> whatever) code would be cool. I will probably have to write some code 
> to get out of this mess, but if someone else has a good starting 
> point, I'm all ears.
>
> Harry, sorry to email you directly about this, but I noticed that you 
> have used PCB to prepare several designs that have gone through 
> manufacturing, and I am interested to hear about your manufacturing 
> experiences. 

A few comments are in order. You definitely don't want to be using 1.6.3 
--- it has some bad bugs that are fixed in the more modern versions. At 
this point, Im recommending using the un-anounced pre-release, 
pcb-1.99j.tar.gz available at:
http://pcb.ece.jhu.edu/pcb-1.99j.tar.gz
I'd hope to finish it into a full release 2.0 quite some time ago, but 
finding enough spare time to work on it is getting very tough lately.

There is a lot of confusion about NC drill file formats. In particular, 
the implied decimal point (# of trailing zeros) seems to vary from 
vender to vendor. Some insist that it match the format in the Gerber 
files (which gerber at least says in the file what it is), others demand 
leading zeros, while others expect the standard: trailing zeros such 
that the last digit is 0.1 mil, but there doesn't appear to be much 
agreement on this. It turns out that the standards document, IPC-NC-349, 
is useless in resolving this issue. My plan (I haven't done it yet) is 
to get rid of zero-suppression altogether and just have large NC drill 
files with leading zeros AND trailing zeros, so that every coordinate is 
six digits long. That will fit the standard, satisfy those demanding 
leading zeros, and satisfy those demanding trailing zeros. What it won't 
satisfy is those demanding equivalence of the gerber and NC file formats 
- - - because the most useful Gerber format violates the NC drill standard. 
I suppose I could bloat the Gerber files with extra leading and trailing 
zeros too and then maybe everyone will be satisfied.

The 1.99j version presently implements trailing zeros.

harry