I was wondering if there was (or we can create) a collection of gerber projects properly set up for fabrication by sparkfun. It would be very helpful if there were several different examples of the ‘right’ way to do things to look at and compare.
Not a bad idea. I’ll need someone else to post correct eagle files but I can post some Protel generated gerbers…
If you still have them, you can use the set of Eagle files I sent with order #6471.
Jake
I have a board if you want, i use an old install of eagle now, means i dont have to worry about changing files.
Perhaps after my exams me and sparky can have a go at sorting the eagle settings file out to get the drills right.
Hey Jake, Ben says your order had the wrong drill file setup :oops:.
Pittuck - You and that school thing. Let me know, I’ve got your DRC/board size tutorial sitting in my inbox.
hehe - they kill us with exams here - must be getting near 18 hours worth now !
sparky:
Hey Jake, Ben says your order had the wrong drill file setup
I readily concede that my FIRST order had the wrong drill file format; but Ben didn’t squawk at my SECOND order. It was the latter that I referenced.
If the second order is also incorrect, then I’m mystified. I looked on the Excellon site and found a detailed definition of the various formats at:
http://www.excellon.com/applicationengi … rogram.htm
Scroll down to the section heading “Leading and Trailing Zeros”
According to my interpretation, and also looking at the sample file on SFE at:
http://www.sparkfun.com/tutorial/PCB/Custom-PCB-FAQ.htm
I still contend that my second file was indeed “2.3 trailing”.
All of us Eagle users are still looking for an example of a drill file, generated by Eagle, that satisfies Ben. Is there such a file? And how will we know for sure?
So Ben, or Sparky, or anyone, please come out of the woodwork and show us a sample of an Eagle drill file that coforms to the SFE requirements.
Jake
Hey Jake,
Ben says that there has never been an eagle 2.3 trailing correct drill file. So we are still in the hunt.
Ben is currently playing with Eagle in hopes of migrating the DRC to a new import.
We’re playing with it, but right now we really need Eagle to output 2.3 trailing to streamline things as much as possible.
-Nathan
Jake, you posted an excerpt of the drill file from your SECOND order in [[this thread](http://www.sparkfun.com/cgi-bin/phpbb/viewtopic.php?t=1235&postdays=0&postorder=asc&start=15) on 15 June 2005. This looks like a 2.3 trailing format to me. Two questions:eejake52:
I readily concede that my FIRST order had the wrong drill file format; but Ben didn't squawk at my SECOND order. It was the latter that I referenced.sparky:
Hey Jake, Ben says your order had the wrong drill file setup
I exported the gerber files using sparkfun’s eagle tutorial(I have v4.14). If my drill file was wrong, Ben diddn’t tell me about it. It was probably wrong, but just diddnt bother to keep telling everyone :). Order #6677
[My DRD File](http://www.paintballelectronics.com/customdm4board.txt)
OK, after two successful .PCB submissions, Ben rejected my third. All three look the same to me and were made w/ eagle 4.11, and import correctly with 2.3 defined into viewmate. Here’s an excerpt, which, of course, looks just like every other .drd file in this thread.
I’m really trying hard, but not sure what the right answer is!
%
M48
M72
T01C0.024
T02C0.032
T03C0.040
T04C0.100
%
T01
X579Y553
X651Y617
X747Y841
X811Y777
X755Y353
X843Y329
X891Y177
X1083Y265
In my last submission (using EAGLE 4.15 with editted eagle.def) I included the following note with the zipped gerber files as suggested by **pittuck**:BigRedBee:
I’m really trying hard, but not sure what the right answer is!
Edit: BigRedBee - do you know that the DRC failure was due to the drill file? Could it have been something else (e.g., minimum spacing, minimum trace size, minimum hole size, etc.)?Created with EAGLE 4.15. Drill file is 2.3 format with LZ suppression.
Don
Yes, Ben specifically identified the drill file as the failing component.
I’ve been playing around w/ Eagle today. I was able to generate a drill file that imports correctly into ViewMate with the following option settings:
Left of decimal: 2
Right of decimal: 3
Omit Trailing Zeros option checked
I also modified the eagle.def (v4.11) file to look like this:
Drill = “X%05.0fY%05.0f\n” ; (x, y)
the .drd file now looks like this:
%
T01
X00579Y00553
X00651Y00617
X00747Y00841
X00811Y00777
X00755Y00353
X00843Y00329
X00891Y00177
X01083Y00265
X01179Y00241
X01131Y00633
X01123Y00681
X01139Y01529
X01051Y01617
X01003Y01721
X00987Y01777
Is this any better?
I just tried this change (note: I already had the resolution fix in place) on version 4.14.
I was able to successfully import a drd into CAMtastic using import settings of “2.3 Trailing Abs Inch” after making this change.
I think BRB just might be onto something here! 
Jerry
yep, mine worked in Camtronix as well, it autodetecs the drill file as 2.3 trailing. I’ll re-submit the job and see how it goes this time.
BigRedBee:
X843Y329X891Y177
X1083Y265
Sparkfun is expecting trailing zeroes to be suppressed, not leading zeroes. It thus interprets those values as:
84.300" x 32.900"
89.100" x 17.700"
10.830’ x 26.500"
I’ll admit I find myself wondering sometimes why people came up with these formats that don’t simply use period to show where the decimal point belongs, but the fact remains that they don’t.
I also wonder why people refer to the formats as e.g. “2.3 trailing” rather than as simply “2.X”, or as “2.3 leading” instead of just “X.3” since what matters in the former case is simply that there are two digits before the decimal point and in the latter case there are three digits after.
Have you re-submitted the job yet? If so, how did it go? Any feedback from Ben?BigRedBee:
I’ll re-submit the job and see how it goes this time.
Don
donblake:
Have you re-submitted the job yet? If so, how did it go? Any feedback from Ben?Don
I re-submitted the job, and got a note back the following Thursdaysaying that the design passed DRC. On Tuesday of the next week (just 4 days later), I got a note saying that by boards had shipped.
Turns out that Sparky fabbed the original set of gerbers that Ben said failed. The boards arrived today.
They look great!