Selecting inches/mm with the RS_274x CAM processor

Michael Sansom schrieb:

Is there any way to output Gerbers files with the RS_274X CAM processor

in anything other than inches?  I'm capturing in mm, so I would think

that the Gerber files would be output in mm, but looking at the files I

can see that I am getting inches instead.  I don't see any place in the

CAM processor dialog to select unit systems.

 

Truly, what I'd really like is a Gerber output in microns (um), but I'll

take mm.  Inches are a problem.

 

Thanks,

 

Michael

Michael,

the default output of Gerber data is in inches. If you prefer to have

"mm" you could change the Gerber device in the eagle.def file or even

better define a new device. That's the place we define the output

devices. It's located in the eagle/bin folder.

Examples for Gerber output in mm 3.3 format:

Type     = PhotoPlotter

Long     = "Gerber photoplotter"

Init     = "G01\nX000000Y000000D02\n"

Reset    = "X000000Y000000D02\nM02\n"

ResX     = 25400

ResY     = 25400

;Wheel    = ""

Move     = "X%0.6dY%0.6dD02*\n"    ; (x, y)

Draw     = "X%0.6dY%0.6dD01*\n"    ; (x, y)

Flash    = "X%0.6dY%0.6dD03*\n"    ; (x, y)

Aperture = "%s*\n"               ; (Aperture code)

Units    = mm

Decimals = 4

Info     = "Plotfile Info:\n"\

           "\n"\

           " Coordinate Format : 3.3\n"\

           " Coordinate Units  : mm\n"\

           " Data Mode         : Absolute\n"\

           " Zero Suppression  : None\n"\

           " End Of Block      : *\n"\

           "\n"

@GERBER_MM_33

Long          = "Gerber photoplotter with automatic aperture wheel

generation"

Wheel         = "" ; avoids message!

AutoAperture  = "D%d" ; (Aperture number)

FirstAperture = 10

Decimals      = 4

Units         = mm

@GERBERAUTO_MM_33

Long          = "Gerber photoplotter with RS-274-X aperture generation"

Units         = mm

Init          = "G75*\n"           \ allow positive and negative coordinates

                "G71*\n"           \ units are mm

                "%%OFA0B0*%%\n"    \ horizonal and vertical OFfset is 0

                "%%FSLAX33Y33*%%\n"\ Format Statement is Absolute (I for

incremental) 3.3

                "%%IPPOS*%%\n"     \ Image Polarity is POSitive (NEG for

nagative)

                "%%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,%6.3f*%%\n"        ; (code, diameter)

Rectangle     = "%%AD%sR,%6.3fX%6.3f*%%\n"  ; (code, dx, dy)

Oval          = "%%AD%sO,%6.3fX%6.3f*%%\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,%6.3f*%%\n"   ; (code, diameter) (looks like

there is no octagon, so we take a circle)

Octagon       = "%%AD%sOC8,%6.3f*%%\n" ; (code, diameter)

Annulus       = "%%AMAN%s\n1,1,%6.3f,0,0\n1,0,%6.3f,0,0*\n"\

                "%%\n"\

                "%%AD%sAN%s*%%\n" ; (code, diameter, inner diameter,

code, code)

Thermal       = "%%AMTH%sX\n1,1,%6.3f,0,0\n1,0,%6.3f,0,0*\n"\

                "21,0,%6.3f,%6.3f,0,0,45\n21,0,%6.3f,%6.3f,0,0,135\n"\

                "%%\n"\

                "%%AD%sTH%sX*%%\n"; (code, diameter, inner diameter,

diameter + 2mil, gap, diameter + 2mil, gap, code, code)

HTH

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

FAQ: http://www.cadsoft.de/faq.htm

Richard Hammerl wrote:

Michael Sansom schrieb:

>> Is there any way to output Gerbers files with the RS_274X CAM processor

>> in anything other than inches?  I'm capturing in mm, so I would think

>> that the Gerber files would be output in mm, but looking at the files I

>> can see that I am getting inches instead.  I don't see any place in the

>> CAM processor dialog to select unit systems.

>>

>> Truly, what I'd really like is a Gerber output in microns (um), but I'll

>> take mm.  Inches are a problem.

>>

>> Thanks,

>>

>> Michael

 

Michael,

 

 

the default output of Gerber data is in inches. If you prefer to have

"mm" you could change the Gerber device in the eagle.def file or even

better define a new device. That's the place we define the output

devices. It's located in the eagle/bin folder.

 

Examples for Gerber output in mm 3.3 format:

snip ....

> snip ....

HTH

 

Thanks,

That worked well.  I reworked it to output in microns (just changed the

scale from what you had by another factor of 1000).  I am bringing

gerber files which are antennas into an RF simulation program that

really wants microns.

Thanks again,

Michael

Hi,

Do I just add the text above in the .def file? Or should I replace anything? I have tried editing the def file by adding but get error messages: Unknown paramter or invalid value

Mags

I'd really like millimetre output to, so I copied/pasted your code above

into teh eagle.defs file, but weird results when I open up the gerber file

(no such problems with the original inch versions)....

http://imageshack.us/photo/my-images/24/30216098.jpg/

It appears just to be the centre line of every track?

Here's the original board layout...

http://imageshack.us/photo/my-images/835/70166729.jpg/

Any ideas?

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

I just copied pasted it into the existing Eagle def file...I received the

same error - it was easy to fix, one of the lines has simply wrapped round

onto a new line (it tells you which line is giving the error) ...therefore

there was no " at the end of the line - I just brought the line that

followed back up to join it where it should have been

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Where should I paste it? Do I need a header or something for the first part, or should it replace something existing?:

Type = PhotoPlotter

Long = "Gerber photoplotter"

Init = "G01\nX000000Y000000D02\n"

Reset = "X000000Y000000D02\nM02\n"

ResX = 25400

ResY = 25400

;Wheel = ""

Move = "X%0.6dY%0.6dD02*\n" ; (x, y)

Draw = "X%0.6dY%0.6dD01*\n" ; (x, y)

Flash = "X%0.6dY%0.6dD03*\n" ; (x, y)

Aperture = "%s*\n" ; (Aperture code)

Units = mm

Decimals = 4

Info = "Plotfile Info:\n"\

"\n"\

" Coordinate Format : 3.3\n"\

" Coordinate Units : mm\n"\

" Data Mode : Absolute\n"\

" Zero Suppression : None\n"\

" End Of Block : *\n"\

"\n"

http://www.webspace.ne.jp/rental/icon_tree_bbs/bbs.php?pid=5574&mode=pr&parent_id=326

Sample for mm 3.4-digit format.

Hi,

This worked just fine for me. (More specifically, this version: http://www.eaglecentral.ca/forums/index.php/mv/msg/34173/117557/ did.)

Is there some reason this isn't in the normal EAGLE distribution? While inches seems to be the most common, I've dealt with a couple of shops that prefer mm.

Thanks!

Brad

 

Is there some reason this isn't in the normal EAGLE distribution? While

inches seems to be the most common, I've dealt with a couple of shops

that prefer mm.

 

Hi Brad,

This is part of the normal EAGLE distribution, at least now anyway ;).

You'll find the drivers listed for EXCELLON_33MM and GERBER_RS274X_33MM.

This was added recently with the release of 7.3 if memory serves.

Let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia