Eagle PCB software - Gerber output setup files

Anything to do with configuring CAM systems and Post Processors to run on different CNC machines

Moderators: Mr Magoo, Martin, bradders, Steve

Post Reply
User avatar
Denford Admin
Site Admin
Posts: 3587
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Eagle PCB software - Gerber output setup files

Post by Denford Admin » Thu 04 Jun , 2009 14:28 pm

A customer with one of our PCB Engravers has configured the Eagle software to create Gerber files suitable for PCB Engraver software's import wizard.

The issue with the Eagle default RS247X output was that units were not defined. Our software defaulted to Metric (%MOMM*%) and it seems Eagle presumed that a default gerber file should be imperial (%MOIN*%)

Zip file includes files:
eagle.def
denford.cam
Attachments
eagle.zip
(9.54 KiB) Downloaded 724 times

iri
Posts: 4
Joined: Tue 16 Jun , 2009 16:38 pm

Re: Eagle PCB software - Gerber output setup files

Post by iri » Wed 17 Jun , 2009 10:54 am

Just found another problem. The mill file is generated as if you are looking from the top, therefore when milling the copper side you have to tell it that it's the component side to get it the right way round. Not too bad except the drill layout is from the top too. This means that you have to mill the copper then turn the board over to drill it. Not good. :cry:

Have you done any double sided boards yet? If so how do you align the two sides?

IAn

User avatar
Denford Admin
Site Admin
Posts: 3587
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: Eagle PCB software - Gerber output setup files

Post by Denford Admin » Wed 17 Jun , 2009 11:03 am

Instead of reading a drill file, try outputting the gerber with un-filled pads where you want to drill.
The software recognises these and will automatically pick out the drill sizes required.
(See attached)
Attachments
un-filled-pads.jpg
un-filled-pads.jpg (152.99 KiB) Viewed 7077 times

iri
Posts: 4
Joined: Tue 16 Jun , 2009 16:38 pm

Re: Eagle PCB software - Gerber output setup files

Post by iri » Wed 17 Jun , 2009 11:14 am

Thanks, that would be the easiest way, but the Eagle CAM processor "Fill Pads" box is permanently checked, and greyed out.
I'm working on that one too!

Just found a button that mirrors the gerber output so that should help.

I think ....

Ian

iri
Posts: 4
Joined: Tue 16 Jun , 2009 16:38 pm

Re: Eagle PCB software - Gerber output setup files

Post by iri » Wed 17 Jun , 2009 11:21 am

According to the Eagle forum there is no way to produce Gerber data with unfilled pads.

Pity.

Ian

User avatar
Denford Admin
Site Admin
Posts: 3587
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: Eagle PCB software - Gerber output setup files

Post by Denford Admin » Wed 17 Jun , 2009 11:34 am

If you can edit the gerber output post, it should be possible to define the "flash" shapes for pads ?

Its a while since I looked at the Gerber file format, but as I remember, pads and tracks are created with basic brush shapes (like potato stamps) called apertures.
They either "flash" a shape into one place (to create a pad for example), or place it and drag it along (to create a track with rounded edges)
The shape of these "stamps" is defined at the top of the gerber file and can contain holes in the middle.
UnFilled pads example wrote:G04 Aperture Table ***
%ADD10C,.100X.040*%
%ADD11O,.100X.080X.020*%
%ADD12O,.080X.100X.020*%
%ADD13C,.040*%
FILLED pads example from same gbr file wrote:G04 Aperture Table ***
%ADD10C,.100*%
%ADD11O,.100X.080*%
%ADD12O,.080X.100*%
%ADD13C,.040*%


If you can modify the post, then it'll be worth looking this up...

iri
Posts: 4
Joined: Tue 16 Jun , 2009 16:38 pm

Re: Eagle PCB software - Gerber output setup files

Post by iri » Tue 30 Jun , 2009 16:19 pm

Thanks, that does make sense. I now remember reading that "doughnut" shapes were used to draw lines, so it must be possible to define them. Maybe I couldn't have unfilled pads because I was using an auto generated wheel file. I have also discovered an Eagle user language program that generates Gcode directly, which I think is what your engraver uses. Last PCB I made worked well, I think the comment about having to drill from the top and mill from the bottom was just my mistake. Onwards and upwards!

Ian

User avatar
Denford Admin
Site Admin
Posts: 3587
Joined: Fri 10 Feb , 2006 12:40 pm
Hardware/Software: Go to User Control Panel > Profile
Enter as much information about your CNC hardware and software as you can - it makes it easier for everyone to know what you're talking about then.
Location: Sunny Brighouse
Contact:

Re: Eagle PCB software - Gerber output setup files

Post by Denford Admin » Wed 08 Jun , 2011 9:00 am

Just been having a go with Eagle and managed to get the Gerber output to work with our Software.
The files given at the top work, but I wouldn't recommend replacing the eagle.def file - you should really edit the existing one and just add a new device by inserting this text at the end of the file:

Code: Select all

[DENFORD_RS274X]

@GERBERAUTO

Long          = "Gerber photoplotter with RS-274-X aperture generation"
Units         = Inch
Init          = "G75*\n"           \ allow positive and negative coordinates
                "G70*\n"           \ units are Inch (G71 for metric)
                "%%MOIN%%\n"       \ String to make Denford engraver read co-ords in INCHES
                "%%OFA0B0*%%\n"    \ horizonal and vertical OFfset is 0
                "%%FSLAX24Y24*%%\n"\ Format Statement is Absolute (I for incremental) 2.4
                "%%IPPOS*%%\n"     \ Image Polarity is POSitive (NEG for negative)
                "%%LPD*%%\n"       \ Layer Polarity Dark (C for clear on negative planes)
                "%%AMOC8*\n5,1,8,0,0,1.08239X$1,22.5*\n"\ Octagons are emulated with a circle (using 8 vertices)
                "%%\n"            ; and therefore the diameter must be enlarged with '1 / cos(pi / 8)'
Reset         = "M02*\n"
Circle        = "%%AD%sC,%6.4f*%%\n"        ; (code, diameter)
Rectangle     = "%%AD%sR,%6.4fX%6.4f*%%\n"  ; (code, dx, dy)
Oval          = "%%AD%sO,%6.4fX%6.4f*%%\n"  ; (code, dx, dy)
; According to the RS-274-X specs there is an aperture macro
; primitive that allows us to specify an octagon (i.e. a polygon with
; 8 vertices). As some Gerber viewers seem to have problems with that,
; we would have to use a round shape for that.
; If your Gerber processor cannot handle the polygon primitive you may
; uncomment the following line and comment out the line after it:
Octagon       = "%%AD%sC,%6.4f*%%\n"   ; (code, diameter) (looks like there is no octagon, so we take a circle)
;Octagon       = "%%AD%sOC8,%6.4f*%%\n" ; (code, diameter)
Annulus       = "%%AMAN%s*\n1,1,%6.4f,0,0*\n1,0,%6.4f,0,0*\n"\
                "%%\n"\
                "%%AD%sAN%s*%%\n" ; (code, diameter, inner diameter, code, code)
Thermal       = "%%AMTH%sX*\n1,1,%6.4f,0,0*\n1,0,%6.4f,0,0*\n"\
                "21,0,%6.4f,%6.4f,0,0,45*\n21,0,%6.4f,%6.4f,0,0,135*\n"\
                "%%\n"\
                "%%AD%sTH%sX*%%\n"; (code, diameter, inner diameter, diameter + 2mil, gap, diameter + 2mil, gap, code, code)
AreaBegin     = "G36*\n"
AreaEnd       = "G37*\n"

Post Reply