Hi Ian (and Alain, and anyone else who is interested), I can confirm that there has indeed been a change made to KiCad concerning the contents of the "Edges PCB" layer within Gerber files (and I was personally responsible for making the change concerned).
Even though you said that your PCB manufacturer has never complained to you about your Gerber files containing the contents of that layer, I still have very good cause to believe that PCB manufacturers, in general, do *not* want the contents of that layer to be included within Gerber files (except of course for the one Gerber file specifically created from that particular layer). As Alain said, I would also seriously suggest that you also generate a Gerber file from the contents of the "Edges PCB" layer, and also provide a copy of that Gerber file to your PCB manufacturer. The contents of that file then stipulate the locations of the edges of your PCB (and hence also stipulate the locations of those edges relative to all of the details contained within each of the PCB's other layers). For your information, note that it actually still is possible to include the contents of the "Edges PCB" layer within the Gerber files for all of the (other) layers. The dialog box now contains an additional checkbox which controls whether the contents of that layer are excluded or included within the other layers, so the state of that checkbox determines what gets included within the (remaining) Gerber files. However, I would strongly suggest that you select the option of including the contents of that layer *only* if your PCB manufacturer specifically requests you to provide such Gerber files (and if you also provide him with a Gerber file created from the contents of the "Edges PCB" layer, which I strongly recommend, he is almost certainly likely to prefer that the remaining Gerber files do *not* also include the contents of that layer). I hope that this infomation is of value to you. I would also have no objections whatsoever to you providing your PCB manufacturer with a copy of this message, should you see any merit in doing that. Regards, Geoff Harland. "Alain M." wrote: > > Hi Ian, > > If I understand you correctly, the new way if correct. I explain: > I already had a board manufactured with that copper line all > around, so it was all short circuited! You were probably giving a > lot of work to your manufacturer to remove that line! > > What I use to do is > 1) send him the board layout, you can even use it to explicitly > specify sizes (when plotting was too expensive, I used to send it > on plain paper) > 2) use alignment targets so that he can fit it all together (you > probably already do this) > 3) I also add two line outside the board (like they use for books) > at each corner. This is easy when the board is a rectangle or not > too complicated > > Alain > > ianf397 escreveu: > > Hi all, > > > > I have successfully been using KICAD for about 2 years, > > initially using version 2006-04-24 on a Pentium 4 running > > Windows XP. > > > > In PCBnew I place the board outline by selecting the "Edges PCB" > > layer, clicking on "Add graphic line or polygon" and drawing the > > board outline. > > > > When the PCB is complete, I run the PLOT (GERBER Format) > > program, and then, when I run the GERBVIEW program I can see the > > board outline in all of the layers. > > I like this, and my PCB manufacturer(PCBTrain) has never > > complained! > > > > However, this week I have installed the newer version of KICAD, > > 2007-11-29-a, and although I do all of the same operations as > > above (I think !), when I run GERBVIEW, I now only see the board > > outline in the "Edges pcb" layer. I don't like this because I > > don't know how the PCB manufacturer knows where the board edges > > are. I don't send the "Edges pcb" file to him anyway. > > > > Please can some kind sole tell me what is happening, is this an > > intentional modification, or has a bug slipped in somewhere ? > > It is, of course, possible that I am doing somethig silly, all > > suggestions are welcome. > > Thanks for your time. > > Regards, > > > > Ian French
