Eagle Drill file flunks DRC

Archive BatchPCB
1

Hi, I’m not sure if I’m ok or not. I flunk the DRC on drill file check -

I don’t have any tool sizes. I’ve followed lots of threads (it would be nice to have this info all in one place, btw). I’m not sure what to do next. Any help would be appreciated. i guess i could hand edit the file but I’d much prefer something reasonably automatic.

Thanks in advance…

Phil

Here’s where I stand:

Using eagle 4.11 on win2K

Modified eagle.def per several threads

Ran silk_gen.ulp

Ran drillcfg.ulp

Downloaded and ran SFE-Special.cam (selected the rack from drillcfg)

Imported the drd to viewmate, changed options per thread (left 2, right 3, omit leading zeros)

Holes line up just fine with the other gerbers.

DRC gives me:

PCB Wizard: Drill File Checker

  • File Uploaded

  • File Read Complete

  • Temporary File Deleted

  • Array Extracted

  • Tools Selections Removed

  • Drill Sizes Extracted [0]

  • Drill Sizes Examined:

FILE DID NOT PASS

Here’s the DRD:

%

T01

X918Y259

X1943Y284

T02

X1331Y534

X1331Y634

X1331Y734

T03

X2031Y697

X2131Y747

X2131Y647

X2031Y597

X2131Y547

X2031Y497

X2131Y447

X2031Y397

T04

X1368Y259

X1268Y259

X518Y344

X156Y359

X156Y459

X156Y559

X156Y659

X156Y759

X518Y824

X518Y664

X518Y504

X1168Y922

X1268Y922

X2181Y922

X2281Y922

T05

X2518Y997

X2518Y122

T06

X281Y259

X281Y859

T07

X2381Y797

X2381Y347

M30

which I believe is not correct, missing tool size following the tool code.

here’s my drill rack

T01 0.024in

T02 0.032in

T03 0.035in

T04 0.040in

T05 0.100in

T06 0.125in

T07 0.128in

Finally, the EXCELLON section of eagle.def

[EXCELLON]

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 = Inch

Select = “%s\n” ; (Drill code)

;Drill = “X%1.0fY%1.0f\n” ; (x, y)

Drill = “X%05.0fY%05.0f\n” ; (x, y)

Info = “Drill File Info:\n”\

“\n”\

" Data Mode : Absolute\n"\

" Units : 1/10000 Inch\n"\

“\n”

It doesn’t appear that tool size is getting printed yet the DrillSize entry seems correct per various threads

2

ok, now I’m feeling confused AND stupid. It turns out that using notepad, I forgot that it defaults to text and saved my changes to eagle.def as eagle.def.txt. sigh. so I wasn’t really using the changes.

however, when I made sure the changes were actually in eagle.def, I get an error on the line

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

comment it out, no error. needless to say, SFE cam job doesn't produce the correct .drd. I'm using Eagle 4.11 - do I need to move up to 14 or 15?

I really don’t want to edit by hand - not because of the work involved but because it’s so error prone.

3

I figured it out. it turns out that cadsoft is a bit loose with their numbering schemes. They claim that 4.1 supports the drillsize option yet 4.11 gives an error. I installed 4.15 and it works correctly (no error, proper drd file and the DRC passes the drill file).

4

ok cool, i was reading, and planning to answer! lol, soo many things to do and so little time to do them.

5

A little more info on this. Cadsoft admitted that their docs were incorrect and said they’d fix them.

Bottom line - Eagle V 4.12 is the first version that implements DrillSize for drillstation devices (i.e. Excellon).

I’d suggest that anyone wanting to use SFEs PCB service get the latest version - 4.16 and add the following entry in the [EXCELLON] section of the bin/eagle.def file:

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