Hi Terry,

I have a dos converter from Lavenir that can convert your Eagle Gerber files
to Protel Gerber file. If you like I can convert them for you and give you
back a Protel 99SE data base.

----- Original Message -----
From: "Terry Creer" <[EMAIL PROTECTED]>
To: "'Protel EDA Forum'" <[EMAIL PROTECTED]>
Sent: Monday, September 29, 2003 4:30 PM
Subject: Re: [PEDA] Eagle to Protel PCB conversion

> 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!
> Thanks,
> TC
> -----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
> >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
> the same as one of the forms that Protel will generate, Protel will be
> 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
> 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
> 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
> place real footprints, the ones that I created in the previous step. It
> 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
> 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
> 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
> difficult to convert into Protel format. This will verify your work, and
> 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