Hi,
I have just completed my first board on Ki-cad, but now I cant send ti to my favorite PCB house, they only use CAM350 and it wont open any of the Gerber files 
I generate gerber using the following settings and open in CAM350 without problem.
The Format 4.5 is important. I once set to 4.6 and some curves on the silkscreen went off board.
Hi,
I dont have cam350 just CamVu… it only wants to open .pcb or .cam files ???
it was these;
Use Auxiliary axis as origin now on
‘include extended attributes’ flag now off
protel filename extentions now off
Format: 4.5
CamVu still cannot see it, but CAM350 is ok now…
It’s probably an old version of CAM350 which doesn’t like the latest Gerber specification and has trouble with arcs. If the PCB house only has an old version of CAM350 it’s time to look for another or nag the fab to get a later version. There’s no point in suffering buggy software when there are so many cheap fabs to choose from these days.
$23 for 10 boards plus $30 delivery… its a fantastic price…
the other fabs are $70-100 extra…
FWIW I have had some problems importing Gerbers into an old version of CircuitCAM (used with an LPKF mill)
If I look at the top of the gerbes produced:
The ones that worked previously have “G04 Gerber Fmt 3.4”
while the new ones that CircuitCAM fails to understand have “G04 Gerber Fmt 4.6”
I would very much appreciate if future versions of KiCad has an option for selecting a legacy Gerber output format. There must be other people with working PCB-manufacturing toolchains from the 1990s or early 2000s that are too expensive or hard to upgrade such as ours. We need the old (e.e. Fmt 3.4) Gerber format.
thanks!
Hm… now that you mention it… I have repeated problems with DirtyPCBs.com’s boardhouse not being able to see my edge.cuts gerber output on their system.
All they see are the drill holes…
The preview on the website is ok, so are all other gerber viewers I tried.
I did found some projects on github where I got access to the gerber files for pcbs in their pcb store - that I assume have been used.
I compared those gerbers with my output and the only difference I could find was:
them
…
G74*
G01*
…
mine
…
G01*
…
Everything else was the same. Even the gerber version.
Currently have a board to make at Dirties and have added the G74* command into my edge.cuts gerber file before the G01* (still loads flawlessly with gerbview after that modification).
So now waiting on the boardhouse again…
If that works it may be worthwhile filing a bug report. Whether or not anyone will act on the bug report is another thing; most devs (including myself) are enraged by software which behaves badly when given a spec. compliant input file and wish producers of such software would either fix their bugs or go out of business. Even UCAMCO plead with implementors to not provide workarounds to other peoples’ buggy software because doing so will create more unnecessary problems for coders.
For anyone having trouble with the current kicad gerbers when they had no trouble in the past, try:
- make sure the “extended attributes” option is off
- remove the “G04 #@!” line from the start of the files; I haven’t traced the logs to see when this was introduced (definitely some time within the past year) but if it’s causing problems it’s pretty easy to cut out in a UNIX shell: sed -i /“G04 #@!.*$”/d .g
1 Like