The problem may not be just limited to protel ascii 2.8 limitations.....

There are a few homebrew options but some may seem more impractical than

1) get a clip file of the allegro board....  write a clip file parser that
handles the recursive LISP like structure of clip language..
NOTE: clip files usually do not transfer test points (I had to learn that
one the hard way and write a PERL script to extract and offset multiple test
points into a clip'ed cut and paste multichannel board to fix that)...

2) export the board to CCT/Specctra router  (allegro v.13 and v.14 make this
easier in File menu)... export wires etc.  Also will need to export pick and
place and make sure origins are same between allegro lib and protel lib. (or
write quickie PERL *.dsn file LISP like parser into ASCII for protel)...
(the netlist info and primitive stuff is in there)....

3) generate allegro artwork... import gerbers into protel... maybe use pick
and place as well... key here is that libraries have to match...
I dunno if the IPC netlisting features will help here or not... plus last I
knew Cadence's IPC netlister had a few bugs...
you can also use a netlist exported from a net_out in Allegro, but you will
need a converter (I used to have a protel-to-allegro netlist munger written
in PERL, but I can't find it... but it wouldn't be too hard to write one
going the other way in PERL).... or you could do the munging with search and
replaces in Word or some such...

then maybe (re)generate/compare netlist from copper... perhaps you would
group pad primitives into components from the gerbers and make pick and
place library matching moot....  (usually a *.dsn would have the primitive
boundaries in it)

4) I'm going from a couple of years ago memory... Don't quote me....  Buy
Cadence's Design Studio (?)... it was on sale for a while (If I recall) for
$4k to $5k USD (much cheaper than protel)... from what I undertand, it
contains OrCad, Specctra (limited to 6 layers... at a time ;-), and
Allegro... I think it was supposed to be Cadence's answer to shrink wrapped
EDA software....

There must be a conversion path from that to Protel (some more convenient
than others)... there may need to be some data massaging but since most of
cadence's things are text file based, it is easier especially with PERL and
knowing a good PERL programmer....   If you have the Allegro *.brd file...
it should convert it to the necessary text as below...

5) purchase said package in (4) or get that company to provide you with

there is an extract utility (I forget the name of it....cds_extract???
allegro_extract???) that comes with the Cadence tools that will directly
read the binary brd file and give you a text file of the extracted
primitives... A PERL script could make breakfast out of that and convert it
to protel ascii

the extract utility uses a text file to describe what kind of information to
extract from the brd file and then generates said output text file...

6) use router solutions inc.

Allegro is super powerful while protel's UI is far superior and makes boards
a joy....

-----Original Message-----
From: Jim McGrath [mailto:[EMAIL PROTECTED]]
Sent: Wednesday, August 15, 2001 5:47 PM
To: Protel EDA Forum
Subject: Re: [PEDA] Alegro Conversion


I don't know what Allegro goes for but the converter I researched was
$11,400 to go both ways. Ouch!

Jim McGrath
CAD Connections Inc.

Bob Jones wrote:

> Hi Jim,
> I guess nobody cares about your Allegro problems!!!!
> What's cheaper the converter or Allegro?
> Bob Jones
> Digitized Technologies
> 2 Summit Road
> P.O.Box 7284
> Prospect, CT. 06712-1541
> Tel: 203-758-6312
> Fax: 203-758-3338
>           [EMAIL PROTECTED]
> Notice:  This message is intended solely for the person to whom it
> is addressed.  Unintended recipients will be legally responsible for
> unauthorized use, disclosure, copying or distribution.  If you have
> received this message in error, please notify the sender immediately
> by replying to this message.  Then delete this message from your
> system.  Thank you.
> ----- Original Message -----
> From: "Jim McGrath" <[EMAIL PROTECTED]>
> To: "Protel EDA Forum" <[EMAIL PROTECTED]>
> Sent: Monday, August 13, 2001 1:37 PM
> Subject: [PEDA] Alegro Conversion
> > Hi All,
> >
> > I have a request from a customer to take in their Alegro PCB files and
> > modify/finish work that has been started in house. I am aware of
> > Router Solutions but have been told it converts to 2.8. Does anybody
> > have practical experience as to the completeness of the conversion
> > and weaknesses/strengths of the conversion?
> >
> > Thanks,
> >
> > Jim McGrath
> > CAD Connections, Inc.
> >

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
* Contact the list manager:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to