My drill file looks like this, and generates a “DRILLS MISSING - NO DRILL FILE HAS BEEN PRODUCED” error when I attempt to run the drill file section of the CAM processor using eagle 4.11
T01 0.020in
T02 0.024in
T03 0.032in
T04 0.040in
T05 0.100in
The error log that pops up contains this information:
Missing Drills:
– Requested –
Size used
0.500mm 6
Drills used:
Code Size used
T02 24.000mil 48
T03 32.000mil 3
T04 40.000mil 13
T05 100.000mil 3
So, I change T01 to it’s metric equivalent, everything passes.
T01 0.5mm
T02 0.024in
T03 0.032in
T04 0.040in
T05 0.100in
I doubt this drill file will fly – any ideas on how to get it to accept the first file?
I’ve run 5 or 6 boards thru batchpcb, so this isn’t likely to be a ‘simple’ mistake on my part…
OK, I’ve decided to create the gerbers with this mixed mode drill file:
T01 0.5mm
T02 0.024in
T03 0.032in
T04 0.040in
T05 0.100in
and then manually edit the drill file to look like this before submitting.
T01 0.020in
On another note, before I bought the registered version of Eagle, I was playing around with an “unlocked” one. Future versions are smart enough to detect this, and prevent you from loading the file. I’ve not found a way around this, and it’s really a pain. Guess I’ve learned my lesson. the painful thing is that, even with a valid personal license, I can’t load my file!
which version of eagle are you using? You will need version 4.15 or later. how are you generating your gerbers? You should be using the cam file SFE-special. It’s around here somewhere - search for it. it gens everything correctly for me but I flailed around before discovering the version issue. (the eagle site said 4.12 would work, nope…).
I’ve been using version 4.11 and SFE-special.cam. I’ve run 4-5 board thru sparfkun, and another 3-4 sets directly thru goldphoenixpcb. THere’s definitely something special about that .020 drill that’s making it act up.
I wish a could upgrade to the later versions, but because of the ‘hack’ the was applied a long time ago, all my design files are ‘poisoned’.
At anyrate, I think I’ve got an interim solution, we’ll see!
BigRedBee:
I wish a could upgrade to the later versions, but because of the ‘hack’ the was applied a long time ago, all my design files are ‘poisoned’.
Greg,
Thinking out loud here, why not ask Cadsoft to fix your files, which where generated by an error (you cetainly wouldn’t have deliberately use a cracked version of their software had you known…)?
If you were to upgrade to the latest version, buy a license, and continue to use their product, I would think they’d clean your old files as a free “good will” service.
BigRedBee:
On another note, before I bought the registered version of Eagle, I was playing around with an “unlocked” one. Future versions are smart enough to detect this, and prevent you from loading the file.
Actually, the “unlocked” version you were playing with detected that it was itself hacked, and purposefully corrupted your EAGLE files. I’ve had this happen, and it’s a pain in the ass, but at least EAGLE makes automatic backups of all your files for you, so it should be relatively easy to recover from (At least it was for me…)
Long story short, don’t even bother trying to use a hacked version of EAGLE…
There is a Legalizer available. A google search or emule search may find the 1.2 version required to recover your schematics and layout.
I’m using the 4.16r version and yeah… the Unlocked version drove me to to the point of not wanting to use Eagle. But its so easy to design a schematic and wireup the layout I persisted.
I haven’t bought it yet, as I’m waiting to see if it’s compatible with the Manufactures before investing the hard earned cash?
I’m about to send off my first pcb, and having no end of difficulty figuring out how to output an Excellon Drill file
The Manufacturer BEC in Brisbane Australia requests the following
Drill files should be Excellon format no. 2 with sizes included in the header.
The preferred format for drill and gerber files is Imperial, 2 integer digits, 3 decimal digits, absolute type with no zero suppression.
Gerber files should be RS274-X . If other formats are used, the file format, integer and decimal digits, aperture table, absolute or relative, metric or imperial and zero suppression settings must be supplied.
Layer files should be generated with a common datum point at 0,0 for all layers. ie do not use auto centre or similar features that place different offsets on different layers.
Top Layer GTL
Bottom Layer GBL
Top Overlay GTO
Bottom Overlay GBO
Top Solder Mask GTS
Bottom Solder Mask GBS
Border for Routing GKO or GM1
Using the SFE Special cam, I just renamed the output file extensions to GTL,GBL etc. But the Excellon output never lines up to the gerber files on ViewMate. The holes are either 90degrees rotated and miles wide or too small and compressed in the bottom left corner?
I’ve tried the modifactions listed I can find here? Is there a way to set the 2,3 no zero supression in eagle? the Cam processor just doesn’t give any options?
Also when selecting Excellon with drill rack (when using drillcfg.ulp) it says missing drills etc.
once you have > 4.15 eagle, make sure you select gerber rs427x as the output device in the cam section.
you need to tell viewmate what format the drills are. I believe the drill file doesn’t describe it’s own format. so go to file/import/drill&route/options/dataformat. it should be obvious from there.
eagle.def in bin defines the device output formats in great detail. somewhere in the sparkfun forums there is a post that talks about editing it but I think 4.15+ default is correct.
Philba, your a legend… I never even saw that option thing in Viewmate. Did everything in there ie 2,3 format and all digits included. Works a treat!
BEC are complaining that they don’t know the file format (ie inches/mm etc) so if I resave the drill file from in viewmate, will it add all the drill and format information needed?
I don’t know what BEC is expecting. The drill file code M72 gets burped out by my eagle/SFE cam job. that says imperial. leading zeros is pretty easy to figure. why don’t you ask them to send you an example of a valid drill file. open it up with notepad and take a look.
edit: run an SFE cam job and open the drd file. if it doesn’t have M72 in first few lines, you should open up your eagle.def, find the excellon section and edit the init line to read this: Init = “%%\nM48\nM72\n”
I believe that’s the default.
also, when I upgraded to eagle 4.15, it decided to use the eagle.def from my earlier installation. that was fun to track down - none of the changes I made did anything. Until I renamed the old .def. That was 2 hours of my life I’ll never get back…
I’ll check it all out and see what BEC can show me as an example file.
Will check that ini value in the def.
They managed to extract the drill data from the converted output to protel I made using the ULP converter. It outputs a binary ASCII protel pcb file. And whilst a couple of the layers were merged. They could generate the drill data file themselves from their protel and use the Gerbers from eagle.
It was a long way round of doing it. and I am assured all will be ok. So, I completed and sent the order in on monday and I should have it either today or monday. Looking forward to that!
Eagle has been fun in that way. If I added up the hours I’ve spent learning and fault finding this software. I reckon I could have gotten pregnant, and given birth it that length of time… which would be a scientific miracle considering I’m a guy!!! oh well, I’m sure generating drill files was easier than giving birth anyway! But not by much!