How do I get an Excellon Drill file with 2.4 precision and trailing zero suppression out of EAGLE?

Question

I'm trying to output CAM data from EAGLE 6.2.0 to get some PCBs made at Advanced Circuits. Their preferred NC drill format (particularly the one used by their online FreeDFM tool) is

Excellon Format, ASCII Odd/ None, 2.4 Trailing Zero Suppression, English Units, No Step and Repeats.

Both their online tool and GC-Prevue are automatically recognizing my NC drill files as 2.3 format with leading zero suppression. So, while the holes are the correct size, they are strewn about an area 10x larger than the PCB, causing the DFM tool to go nuts and I'm about ready to follow.

Can I get EAGLE to give me 2.4 trailing-suppressed files (or maybe at least no suppression)? Or, is there a tool that can convert the mangled files EAGLE vomits out to something reasonable?

I've tried using the 'hack' described here in attempt to force no zero suppression, but then my files are detected as 3.3 precision.

My CAM job is defined as:

[Sec_8]
Name[en]="Drill File"
Prompt[en]=""
Device="EXCELLON"
Wheel=""
Rack=""
Scale=1
Output=".NC"
Flags="0 0 0 1 0 1 1"
Emulate="0"
Offset="0.0mil 0.0mil"
Sheet=1
Tolerance="0 0 0 0 0 0"
Pen="0.0mil 0"
Page="12000.0mil 8000.0mil"
Layers=" 44 45"
Colors=" 1 2 1 2 1 2 1 2 1 2 1 2 1 2 1 2 6 6 4 8 8 8 8 8 8 8 8 8 8 8 8 8 4 4 1 1 1 1 3 3 1 2 6 8 8 5 8 8 8 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 4 2 4 3 6 6 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 0"

Answer 1

Change Device to "EXCELLON_24".

Here are some lines from a .XLN using Device="EXCELLON_24":

...
T01C0.0130
...
T01
X13969Y11517

And here are those same lines in the wrong format using .XLN for Device="EXCELLON":

...
T01C0.01300    
...    
T01    
X139686Y115173

This wrong format causes the 10x NC Drill error shown above; I did not check this with GC_Prevue, but I saw this 10x problem when uploading to OSHPARK.

Answer 2

Can you post the NC Drill section of the CAM file you're using? I've made several successful orders from Advanced Circuits and always check FreeDFM. I'm on Eagle 6.3.0 right now, but I've been using the same CAM file for a while.

This is the NC Drill section from my CAM file for AC's standard four-layer (unless you blind &| buried vias, this should work for any number of layers):

[Sec_9]
Name[en]="NC Drill"
Prompt=""
Device="EXCELLON"
Wheel=".whl"
Rack=""
Scale=1
Output="%P/CAMs/%N/NC_Drill.drp"
Flags="0 0 0 1 0 1 1"
Emulate="0"
Offset="0.0mil 0.0mil"
Sheet=1
Tolerance="0 0 0 0 0 0"
Pen="0.0mil 0"
Page="12000.0mil 8000.0mil"
Layers=" 44 45"
Colors=" 1 2 1 2 1 2 1 2 1 2 1 2 1 2 1 2 6 6 4 8 8 8 8 8 8 8 8 8 8 8 8 8 4 4 1 1 1 1 3 3 1 2 6 8 8 5 8 8 8 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 4 2 4 3 6 6 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 0"

You'll probably want to change the output since that one puts it in a sub-folder. Otherwise, give it a go.

Answer 3

Probably I found a cause of that problem as I just faced it. The coordinates in your drilling file (*.TXT usually) are ten times larger than they should be most likely because the resolution of a device used in CAM processor (EXCELLON most likely) is 10 times higher than the resolution for GERBER_RS274X. To check it, try the following:

Open the file eagle.def in your $EAGLEDIR$\bin and find a section related to the device you used for drilling file generation, I'll show mine for EXCELLON:

[EXCELLON]

Type     = DrillStation
Long     = "Excellon drill station, coordinate format 2.5 inch"
Init     = "%%\nM48\nM72\n"
Reset    = "M30\n"
ResX     = 10000
ResY     = 10000
;Rack     = ""
DrillSize  = "%sC%0.5f\n"        ; (Tool code, tool size)
AutoDrill  = "T%02d"             ; (Tool number)
FirstDrill = 1
BeginData  = "%%\n"
Units    = Inch
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             : 1/100000 Inch\n"\
           "\n"

Now, notice ResX and ResY parameters. When I got 10x larger files than expected, these rows contained 100000 constants. I reduced them to 10000 and voila, I got what I expected.

Also please note that instead of reducing EXCELLON resolution you may want to increase GERBER_RS274X resolution, depending on your needs/board/board manufacturer.

Answer 4

In GC-Prevue, from the menu select Tools/Customize; Select Settings tab; Tick Use Default NC Drill Import Parameters; Press the button to the right to set the defaults and set Whole Digits to 2 and Precision to 4

HtH Dave