Hello dear KiCad community,
I am a very new KiCad user switched from eagle because of the limitation of the boardspace in the free eagle version.
I successfully designed a board and now want it to be made. With eagle I used pcb-pool.com for manufacturing the board which is very easy made by just uploading the .brd file to pcb-pool.com. But after designing the board with kicad it seem like pcb-pool cant handle the new .kicad_pcb files and wants to have the old version .brd files instead.
After some time of unsuccessfull searching for a way to convert the .kicad_pcb file to .brd I would like to ask you whether you know a smart solution for this problem? Is there a convert button I dont see? At least I would be very glad about such a feature!
(I already searched through this forum but only found the solution to convert the .kicad_pcb file by hand with an editor. At a first look at the two file types in textform I skiped this for the moment )
The magic word is Gerber.
Search for the plot button in pcbnew and hit it… then set the output formats according to what Eurocircuits accepts in Gerber…
Usually you want to use something like the following to make it work, but take it with a bag of salt as I don’t use Eurocircuits (dialog options are per KiCAD r6098):
plot format: gerber
Edge.Cuts (rename extension to GML or GBR, dont use GKO!)
B.Paste (for stencil)
F.Paste (for stencil)
Exclude PCB edge layer from other layers
Use Protel filename extensions
Include extended attributes
default line width (mm):
drill map file format:
drill file options:
deselect ‘merging of PTH and NPTH’ if needed
Oh, and for housekeeping I suggest you use a sub-directory in your project folder (I call mine just ‘gerber’) and let the plot tool use that as output as this way you don’t get confused with all the other project files what needs zipping for the manufacturer.
Oh, and use the gerbview tool that comes with KiCAD to check the plot output. If you want another opinion you can also download and install GC Prevue (2D viewer similar to gerbview) or ZofzPCB (nice 3D, similar to pcbnew). Then there is online circuitpeople.com (shows each layer separate, not drill files) or mayhewlabs.com/webGerber (drill output for that to show correctly needs to be ‘keep zeros’ instead of ‘decimal’, doesn’t take outlines no matter what I do) and finally… Eurocircuits very own PCB visualizer (you see it once you upload your files).
What the heck, here a little test I did 2 days ago… all Gerber.
Out of curiosity why don’t you want to use GKO? That is the standard board keepout layer that I use to define all of my board edges when I order boards, I find most board houses actually prefer that format.
Is there a gotcha with Kicad Edge.cuts I don’t know about?
Sorry, I just copied my own KiCAD settings rules in there - if the boardhouse demands the outline to be on GKO, then sure, name it like that. It’s just a file extension, the files looks the same on the inside, as per the Gerber specs only GBR is registered anyway.
GKO stands for gerber keep out and defines something for pick&place machines afaik and something like GML (mechanical layer) or the plain GBR should be more fitting.
Normally if one uploads there is a dialog there where you can check/assign the meaning of your files to what the boardhouse automat think they are.
Anyhow, that’s why I put that bit with the bag of salt in the front of that advice up there.
The following list is copied from the net - seems it’s more some kind of we-do-it-like-that-Protel-thing:
.txt - Drill file
.gbl - botom layer
.gbs - bottom solder mask
.gbo - bottom overlay (silk screen)
.gbp - bottom paste
.gko - keep out
.gm1 - mechanical 1 (board outline)
.gm2 - mechanical 2
.g1 - inner routing layer 1
.g2 - inner routing layer 2
.gp1 - inner plane 1 Negative
.gp2 - inner plane 2 Negative
.gpb - bottom pad master
.gpt - top pad master
.gtp - top paste
.gtl - top layer
.gts - top solder mask
.gto - top overlay (silk screen)
Other Miscellaneous Files:
.rul - rule report file
.ldp - layer report file.
.apr - aperture report file
.drl - unknown binary drill file
.drr - drill report
I use protel for work, which explains why I do that. I thought maybe you were advising of some potential issue with board houses/kicad if it was re-named to .gko
Thank you for your answers Joan_Sparky and Ldoiron17! The Gerber files were exactly what I was searching for.
I had some problems to get them into pcb-pool.com but eurocircuits handled them without any problems.
The problem is solved, thanks again for the help.
would you mind to share the pcb edge with some footprints? (no need to have the nets inside)
I’m improving my StepUp tools, adding a GUI to import directly the .kicad_pcb board and I would like to test if I can manage all cut-outs and the drills used for breaking the pcbs…
edge cut lines had been done in Inventor (as Sheetmetal) and imported into KiCAD as DXF.
I cleaned up anything unimportant from the file - fits just onto a 10x10 cm2 pcb - thickness should be 1mm so one can assemble this.
9-GON-FRAME.zip (9.2 KB)
i am using the daily builds of Kicad for about a year now - and pcb-pool is fine with the new format!
just add a readme in the zip you upload where you write down what KiCAD version you are using!
sometimes the will ask again. but in about 90% its all fine and you will just get your board made
and to make it a step easier i have setup a KiCAD template with the pcb-pool specifications predefined:
template_PCBPool_20160121.zip (6.7 KB)
thank you for our reply! Since I had problems with pcb-pool I switched to eurocircuits. With eurocircuits and the KiCAD gerber files everything works perfectly and I am really pleased with that. But thank you anyway for your answer!