At 05:57 PM 7/27/2005, Harry Selfridge wrote:
You can't import the "holes" into the PCB editor in any way that will help you with the thru-hole pads. What you are trying to do is called reverse engineering.
I've been called upon to reverse-engineer from gerbers. Generally, by the way, this is not piracy reverse-engineering; rather it happens where the design files have gone missing.
I've never done it with Protel, but with Tango I wrote a utility to take drill files and import the drill information to a Tango PCB file which had pads only. Essentially the utility would take a drill size and position and look for a pad at the same location, and if the pad was found, the pair of surface pads at the location (that's the usual case) were converted to a single pad with the appropriate hole.
This could be done fairly easily in a spreadsheet, if one doesn't want to write a utility. You'd need to extract the drill sizes and locations from the drill file -- not difficult, the standard format is very simple --, correct for offset variation between the drill file and layer gerbers, and then sort the information from the PCB file that you created with the gerber imports by location, together with the holes sorted by location. Then it is a matter of creating some formulas to copy the holes into the PCB pad fields, convert at least one of the pads to a through-hole pad, and tag the redundant records for deletion; then the spreadsheet would be imported back into Protel.
There are details that need to be understood to accomplish this: essentially one needs to know how to use the spreadsheet facility of P99SE. Given that, and having good skills with spreadsheets in general, it is not difficult.
And more reliable than using global edits based on an assumed relationship of pad size and drill size.
Another approach, simpler to do but which would take longer for a large board, would be to convert the drill data into simple gerber data. I'd use a flash per drill hit, with the diameter of the flash being the hole size. (Again, gerber format for this is trivial to understand, a little experimentation and you'll get it. Drill data is generally sorted by drill. So for each drill, when the command comes, I'd substitute an aperture. Then the location data can be converted into the very similar data in a gerber file. That's it. Then this drill gerber would be imported into the pcb file, perhaps on the drill layer. I'd then globally edit these pads so that they have a Net assignment equal to the diameter, and I would copy them to the bottom layer, say.
I would then use Nets Reconnect to assign the pad nets net to the associated bottom pad. (I would do this in a PCB that only had bottom pads in it, not tracks). I would then use global edit to edit, for each hole size, all bottom pads with each different net assignment to have that hole size, but *not* for pads with net equal to pad diameter. As I did this, I would delete each set of pads on the bottom layer that came from the drill layer.
As I did this, I could at any time see quickly what pads remained to be converted. And at the end, I could easily check that the final pads have the right holes by displaying the layers appropriately. Then I could delete all the pads on the drill layer.
It probably takes almost as long to describe as to do.... except for the first step, figuring out how to convert drill data to gerber data.
We could do this, by the way, if anyone needed the service and didn't want to hassle figuring it out.
Abd ul-Rahman Lomax LOMAX DESIGN ASSOCIATES PCB design, consulting, and training Protel EDA license resales Easthampton, Massachusetts, USA (413) 527-3881, efax (419) 730-4777 [EMAIL PROTECTED] ____________________________________________________________ You are subscribed to the PEDA discussion forum To Post messages: mailto:[email protected] Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[email protected] Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[email protected]
