I am getting ready to create prototypes and after exporting to Gerber format I get the following error from the manufacturer I have chosen:
“This PCB is missing a board outline file (.bor). Board dimensions have been automatically calculated from the available layers. You must provide a valid board outline file prior to verifying part placement or ordering this PCB”
I have absolutely stalled at this point. It must be something simple I’m doing but I can’t understand it. I don’t know where to start to create this file??
Same problem with most manufacturers. How do you guys send this stuff out to manufacturer without the proper gerber files? I am confused. It has to be on me, I am just not sure what I’m doing incorrectly.
Are they in GerbLook.
http://gerblook.org
It sounds like the PCB board is missing.
The bord outline is the ???_contour.gm1, I have had several boards fabricated and never had a problem…
What pcb shape are you using?
I am using a standard rectangle board around 100mm x 50mm. Nothing super special.
I will check it in Gerblook and see if the contour.gm1 file is there and report back.
Thank you to you both for starting me off on where to look!
So it looks ok in Gerblook more or less.
The contour file is indeed present.
Here is the error: two different apertures share the same D-code
Here is what is in my contour file:
G04 MADE WITH FRITZING*
G04 WWW.FRITZING.ORG*
G04 DOUBLE SIDED*
G04 HOLES PLATED*
G04 CONTOUR ON CENTER OF CONTOUR VECTOR*
%ASAXBY*%
%FSLAX23Y23*%
%MOIN*%
%OFA0B0*%
%SFA1.0B1.0*%
%ADD10R,3.937010X2.362200*%
%ADD11C,0.008000*%
%ADD10C,0.008*%
%LNCONTOUR*%
G90*
G70*
G54D10*
G54D11*
X4Y2358D02*
X3933Y2358D01*
X3933Y4D01*
X4Y4D01*
X4Y2358D01*
D02*
G04 End of contour*
M02*
I have no clue where to go from here. At this point I am completely lost.
I have no clue about Gerber production, because I make my own, but it sounds like something is on top of another.
We’ll have to wait for some expert.
What company is complaining about the board.
EDIT
Did you run the DRC check in FZ.
Thanks for the input Old_Grey, I think I have made progress.
Many companies (not one) are complaining about the problem with the Gerber border file. So it is something in Fritzing for sure.
Here is what I have figured out:
IF I choose a different PCB (curved edge, elliptical etc) it works.
IF I choose the generic rectangle PCB it fails.
So there seems to be a problem with the rectangle PCB choice at the end of the day.
Maybe delete that rect PCB and add a new one.
Lots of people’s stuff seam ok so it might be something in the .fzz
This is someones that works.
http://gerblook.org/pcb/TDDAmLYGorUtXnieQ3GwCH
I have actually tried a new fresh install, and brand new mock-up drawings on Windows, Mac, and Linux, they all fail the same way.
Because the common thread is me, and something I could be doing “wrong”, I am not prepared to say it is a bug yet.
I have in fact deleted the PCB many times, and dragged it over from parts appropriately and then the failure continues.
For this prototype, rounded corners won’t kill me, but in the long run I need to be able to use rectangle.
More information:
The GM1 file is truncated when a rectangle shape is chosen. This truncates on any O/S or install I try .
With a rounded corner PCB for example, the length of GM1 files is 109KB but when using the normal rectangle choice it is 370 Bytes which is basically nothing.
I am now fairly certain this is a bug but will keep testing, but something is truncating the file. This was apparently a previous bug as well as I found a bug report for it.
So it is a bug, and I can repeat it over and over again on several machines. It only happens with rectangle. All the other types work (Arduino shield for example).
Compound that with the inability to get out a proper BOM from the software (sadly, HTML “Shopping lists” are not BOMs) and I am unable to send off anything to manufacture. Most manufacturers (in-fact just about all) require some sort of centroid list (XYRS or something of the kind) so I think my time with Fritzing has come to an abrupt end.
It’s too bad because I really LOVE this software. I have some previous experience with Eagle and it has nothing on the easy and speed of Fritzing. Unfortunately Eagle outputs the files in the right format for manufacture and Fritzing simply does not. I found a few things on the forums asking about a proper BOM etc and there doesn’t seem to be an answer. I would say Fritzing is good if you want to do a breadboard, nice and visual. Maybe you can get a PCB built too but you won’t be sending anything over to really be built.
Overall I would say Fritzing is the product that could still be great if a few things were fixed, but looking at the dev cycle that seems unlikely.
I appreciate everyone’s help here! I like community based projects.
You can make any size, shape, color, and opacity PCB you like. I draw all my boards up and seldom use the ones that come with FZ. (see attached), for some reason .svg cannot be uploaded to this forum so we just zip them up into an .fz… which is just a zip file. Unzip the attached an load in the 100mm x 50mm board though the Inspector (load image file)… Rectangle-pcb_100mm-50mm.fz (721 Bytes)
Thank you steelgoose!
That seems to work. It is just the “generic” file that comes with Fritzing that is the problem it seems. Making your own works great, I had no idea you could do that with just the right .svg file.
Seems like the only problem for me now is the BOM which is a show stopper.
I will continue to watch Fritzing with great hope 
I think the FZ rectangle PCB may be script generated… it may also be missing the ID:“boardoutline”…
What is the problem with the BOM?
That explains maybe why the “generic” rectangle doesn’t work. Using my own now and it’s perfect. It is that file that comes by default that is the problem.
The BOM is not formatted properly for any full integrator that I have found (manufacture the pcb, supply parts, place parts etc). The placements in the pnp file are missing some orientations etc and the BOM is not in a format that anyone takes that I have found (perhaps some do, I just haven’t found any).
For manufacture you need a centroid/XYRS file for pick and place. Now, some places will in-fact process the Gerber files and create the centroid files for you (for a fee).
Here is a really simple example: http://i.screamingcircuits.com/docs/SampleCentroidFile.txt
Most software like KiCad, Eagle, Altium etc all output centroid files to send straight to manufacture. BOMs in CSV or XLS files are often accepted if formatted correctly but then getting that BOM to the actual floor requires the centroid file.
Thank you so much for all the input
I am familiar with Eagle and will use that until Fritzing matures some more.
I really think Fritzing is the way of the future but it has a long way to go, and that is OK! Overall Fritzing is excellent for breadboard work and good to get people in to simple designs.
I’m looking forward to more from Fritzing.
I recommended to a colleague today to use Fritzing for his breadboard lab work. He could then make a nice schematic from it. From there he can re-draw the schematic in Eagle (I always believe in two draws = 1 production run). Then in Eagle he can lay out the PCB, output the needed manufacture files and send if off to any number of places in the U.S., Malaysia or China for manufacture.
There seams to be the misconception that Fritzing should be among the ranks of Eagle, Altuim, Diptrace, and other commercial EDAs. Fritzing is and open source educational tool to help makers (both young and old) to get acquainted with the wonderful world of today’s electronics… Fritzing does what it was design for; teaching the relationship between your schematic, breadboard prototype, and then making your prototype on a PCB… either DIY or by a prototype PCB fabrication service. Fritzing has filled a gap in the Arduino revolution… with today’s high-tech PCB manufacturing equipment you can buy commercial quality PCBs at just a fraction of what it would have cost just a few years ago and affordable to everyone, and Fritzing helps make that possible… Comparing Fritzing to Eagle is like comparing Arduino or Energia IDEs to IAR or Kile… you are not going to write commercial firmware for a ARM Cortex processors with Energia… the tools just are not there for writing commercial firmware…
Use the right tool for the right job… for what you want to do you should be using one of the commercial EDAs… and for creating centroid files for an assembly house, Eagle is a good choice…
