Abd ul-Rahman,
                Thanks for taking the time to reply! Ill try playing around
with the file tonight. Thank god it's a relatively small double sided PCB
and not an 8 layer monster!



-----Original Message-----
From: Abd ul-Rahman Lomax [mailto:[EMAIL PROTECTED]
Sent: Tuesday, 30 September 2003 8:36 AM
To: Protel EDA Forum
Subject: Re: [PEDA] Eagle to Protel PCB conversion

At 02:15 AM 9/29/2003, Terry Creer wrote:
>Hi All,
>         I acquired a PCB done in Eagle and I want to modify it with Protel
>99SE. What's the best way to achieve this? Can I do it somehow with the
>freeware version of Eagle? By Gerber maybe?

Gerber is the Swiss Army Knife of file conversion. Since Eagle will 
generate Gerber and Protel will import Gerber, it *can* be done.

So, assuming you can get or generate the Gerber, perhaps from a demo or 
freeware version, or from an accomodating Eagle licensee, you then need to 
massage the Gerber into Protel-readable form. It's been a while since I've 
done this, but I would take a look at some Protel-generated Gerber.

There are a lot of ways to write Gerber and Protel can only read some of 
them. Protel requires, as I recall, that certain headers be present. The 
short of it is that if you output or massage the gerber into a form that is 
the same as one of the forms that Protel will generate, Protel will be able 
to read it.

Note that Protel does not support all of the flash shapes....

(To massage Gerber, I've often used Excel. You can take a file, massage it 
into Tab delimited fields with Word, then take it into Excel. At this 
point, for example, if you wanted to take incremental gerber into 
fully-explicit absolute no-zero-suppression gerber, you could insert fields 
as necessary, format the numbers, etc.)

Anyway, assuming you can load the Gerber into Protel, here is a process 
that I might use to do the conversion.

In Eagle, I'd take the PCB and delete everything except one instance of 
each footprint to make a file I'll call Footprint. I'd generate a report on 
this showing the footprint names. I'd plot this board, take the plots into 
Protel, and then create footprints for each original.

The I'd take the original Eagle PCB and generate two sets of plots: one 
with just the footprints and one with just the non-footprint primitives. 
I'd bring the first set into Protel onto mechanical layers and use these to 
place real footprints, the ones that I created in the previous step. It may 
be possible to automate this step if Eagle will generate a pick-and-place 
report. This report may be massaged into proper form to drive the Protel 
place-from-file process. If the board is simple, it may not be worth the 
effort, but if it is complex, then the work necessary to make the rotations 
for the parts correct, etc., may be well worth it.

(PCB/Tools/Autoplacement/Place from File. This uses a Protel PIK file to 
autoplace components....)

Then I'd import the tracks and vias; gerber batch import should put them on 
the proper layers. The pads that come in at this point -- Protel imports 
flashes as pads --, you may want to convert to vias (Tools/Convert).

You'll also want a net list from the original board. This too should be not 
difficult to convert into Protel format. This will verify your work, and is 
essential if you have power planes, etc., since imported gerber will *not* 
create a proper Protel inner plane, which is net-driven.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to