Metric CAM (excellon/gerber) files

Andy Warner schrieb:

I am designing a metric board, can I generate cam files

that are also metric, if so how ? It seems that the excellon and gerb274x

cam files generate inch-based outputs. Do board houses

even accept metric cam files ?

 

If conversion to inches is not necessary, I would

like to avoid it, for all the obvious reasons.

--

Andy

It's possible to change the definition of the Gerber device in the

eagle.def file or even add further devices.

For example, Gerber in MM, data format 3.3:

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

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,%6.3f*%%\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)

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

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

"Richard Hammerl" <ric@cadsoft.de> wrote in message

news:gk4fq1$tqm$1@cheetah.cadsoft.de...

It's possible to change the definition of the Gerber device in the

eagle.def file or even add further devices.

 

For example, Gerber in MM, data format 3.3:

 

Thanks, I'll try that tomorrow - much appreciated.

Here's what I had hacked together (untested) for a metric excellon

device to generate .drd files:

Type     = DrillStation

Long     = "Excellon drill station"

Init     = "%%\nM48\nM72\n"

Reset    = "M30\n"

ResX     = 1000

ResY     = 1000

;Rack     = ""

DrillSize  = "%sC%0.4f\n"        ; (Tool code, tool size)

AutoDrill  = "T%02d"             ; (Tool number)

FirstDrill = 1

BeginData  = "%%\n"

Units    = mm

Select   = "%s\n"                ; (Drill code)

Drill    = "X%1.0fY%1.0f\n"      ; (x, y)

Info     = "Drill File Info:\n"\

           "\n"\

           " Data Mode         : Absolute\n"\

           " Units             : 1/1000 mm\n"\

           "\n"

Is that adequate, or do you have a better suggestion ?

I'm looking forward to banishing inches from my process.

--

Andy

Andy Warner schrieb:

 

"Richard Hammerl" <ric@cadsoft.de> wrote in message

news:gk4fq1$tqm$1@cheetah.cadsoft.de...

It's possible to change the definition of the Gerber device in the

eagle.def file or even add further devices.

 

For example, Gerber in MM, data format 3.3:

 

 

Thanks, I'll try that tomorrow - much appreciated.

 

Here's what I had hacked together (untested) for a metric excellon

device to generate .drd files:

 

 

Type     = DrillStation

Long     = "Excellon drill station"

Init     = "%%\nM48\nM72\n"

Reset    = "M30\n"

ResX     = 1000

ResY     = 1000

;Rack     = ""

DrillSize  = "%sC%0.4f\n"        ; (Tool code, tool size)

AutoDrill  = "T%02d"             ; (Tool number)

FirstDrill = 1

BeginData  = "%%\n"

Units    = mm

Select   = "%s\n"                ; (Drill code)

Drill    = "X%1.0fY%1.0f\n"      ; (x, y)

Info     = "Drill File Info:\n"\

          "\n"\

          " Data Mode         : Absolute\n"\

          " Units             : 1/1000 mm\n"\

          "\n"

 

Is that adequate, or do you have a better suggestion ?

 

I'm looking forward to banishing inches from my process.

--

Andy

You still have to change the resolution. Set

ResX     = 1000

ResY     = 1000

to

ResX     = 25400

ResY     = 25400

This means you male 25400 steps per inch. Which results in a

resolution of 1/100 mm.

HTH

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

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

"Richard Hammerl" <ric@cadsoft.de> wrote in message

news:gk727q$ean$1@cheetah.cadsoft.de...

ResY     = 25400

 

This means you male 25400 steps per inch. Which results in a

resolution of 1/100 mm.

I think I have edited eagle.def correctly now to include mm 3.3

excellon and gerber devices. Do I need anything funky to the .cam

files ? They seem peppered with inch-based detail too.

The gerbers look OK in my gerber viewer, when I just copy

the excellon and gerb274x .cam files and reference the corresponding

MM33 output device.

Andy Warner schrieb:

"Richard Hammerl" <ric@cadsoft.de> wrote in message

news:gk727q$ean$1@cheetah.cadsoft.de...

ResY     = 25400

 

This means you male 25400 steps per inch. Which results in a

resolution of 1/100 mm.

 

I think I have edited eagle.def correctly now to include mm 3.3

excellon and gerber devices. Do I need anything funky to the .cam

files ? They seem peppered with inch-based detail too.

 

The gerbers look OK in my gerber viewer, when I just copy

the excellon and gerb274x .cam files and reference the corresponding

MM33 output device.

You don't have to change anything in the CAM files. Simply use

the Devices you have changed.

--

Mit freundlichen Gruessen / Best regards

Richard Hammerl

CadSoft Support -- hotline@cadsoft.de

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

Andy Warner wrote on Mon, 05 January 2009 12:37

I am designing a metric board, can I generate cam files that are also

metric, if so how ?

What units you used to size the board and define the packages on that board

have nothing to do with how the resulting information is written to Gerber

files.  Most boards require a mix of units for various parts anyway.

Quote:

It seems that the excellon and gerb274x cam files generate inch-based

outputs. Do board houses even accept metric cam files ?

 

If conversion to inches is not necessary, I would like to avoid it, for

all the obvious reasons.

There is no "conversion" to worry about since how you got to the

measurements has nothing to do with how they are written to CAM files.  And

no, your objection is not obvious at all.  I would leave the defaults

alone.  Board houses know how to interpret these files.  I wouldn't send a

board house a metric Gerber file unless they specifically told me they can

handle it.  No board house is going to misinterpret a inch file.  I'd be

more worried that their process assumes inch files and therefore

misinterpret metric ones.

Keep in mind that inside Eagle it's really neither inches nor mm.  If I

remember right, they use integers of some very small unit.  But all that

doesn't matter.  The computer will convert.  Computers are good at that

sort of thing.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Olin wrote on Tue, 02 March 2010 22:07

There is no "conversion" to worry about since how you got to the

measurements has nothing to do with how they are written to CAM files.

And no, your objection is not obvious at all.  I would leave the defaults

alone.  Board houses know how to interpret these files.  I wouldn't send

a board house a metric Gerber file unless they specifically told me they

can handle it.  No board house is going to misinterpret a inch file.  I'd

be more worried that their process assumes inch files and therefore

misinterpret metric ones.

Maybe he read Olimex's FAQ which says:

Quote:

Q: I designed my board in Inch (mm) units, in which units should I

export my Gerbers?

A: Always export your gerbers in the units you designed board to

prevent rounding errors in your Gerber generation due to the unit

conversion.

which would make it obvious to not want to make gerbers in inch when the

board is made in mm. But, what do I know...

Stig

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Maybe this doc is of relevance to your Q

http://www.artwork.com/gerber/274x/rs274xrevd_e.pdf

Table 1, page 9 shows there are codes to select inch or mm units. Eagle's

CAM processor does inch all the time afaik.

StigOE wrote on Wed, 03 March 2010 02:41

Maybe he read Olimex's FAQ which says:

Quote:

Q: I designed my board in Inch (mm) units, in which units should I

export my Gerbers?

A: Always export your gerbers in the units you designed board to

prevent rounding errors in your Gerber generation due to the unit

conversion.

That is both silly and misleading.  Olimex is hardly the board house to

listen to.  They are the only board house I've ever encountered that wanted

files different from what every other board house was happy with.  (In

addition they had a uppity attitude about it and tried to make it look like

I was a criminal for even asking for a quote.  Fortunately there are better

board houses out there, so there's no need to put up with that sort of

crap.  I use Gold Phoenix for most of my prototypes, for example.)

In addition to that, I thought I read somewhere but can't find now that

Eagle stores coordinates internally as integers of some very small unit.

Your board isn't inherently in mm or inches anyway.  I think the small unit

was deliberately chosen so that integer multiples would get to both a small

round fraction of a mil and a mm.  Even if not, any roundoff error will be

so small as to be irrelevant since the CAM processor write extra digits for

this reason.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca