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:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to