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.
Mike, ----- 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 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: * mailto:[EMAIL PROTECTED] * * Forum Guidelines Rules: * http://www.techservinc.com/protelusers/forumrules.html * * Browse or Search previous postings: * http://www.mail-archive.com/[EMAIL PROTECTED] * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
