In spite of my attempts to follow all the rules, I’m in the drillfile doghouse because my drill file wasn’t quite right. The message I got from SFE was “In the future … export your drill file in 2.3 trailing suppression format.”
I am using Eagle V4.14, I used SFE_special.cam to generate the file, and I checked it with Viewmate. I also read all the FAQs, tutorials, and most of the forum posts. So where was the glitch? Can someone help please.
Jake
Here is the first few lines of the file that got me in the doghouse:
%
M48
M72
T01C0.0320
%
T01
X1423Y1927
X1423Y2927
X1423Y3927
X2423Y3927
I found that the file eagle.def, in section [EXCELLON] has entries that look like sprintf() strings, that control the way the above lines are printed. Specifically:
DrillSize = “%sC%0.4f\n”
controls the line T01C0.0320
and this one
Drill = “X%1.0fY%1.0f\n”
controls the the other lines like X2423Y3927
BUT
ResX = 10000
ResY = 10000
also controls the resolution of the X & Y coordinates.
Is this the right place to be messing?
Has anyone come up with a good solution?
Jake
Jake, I believe this is the problem. I've done one Spark Fun PCB successfully. This section of my eagle.def file is:eejake52:
BUTResX = 10000
ResY = 10000
also controls the resolution of the X & Y coordinates.
If you're using ViewMate to view the drill file, note that ViewMate defaults to 3.4 mode. Before you import the drill file, click options and change the format to 2.3.ResX = 1000
ResY = 1000
Don
so just to confirm the sparkfun cam fIle does work???
Pittuck> “so just to confirm the sparkfun cam fIle does work???”
It generates the gerber files fine (top and bottom traces, solder mask, silk screen); but it doesn’t appear possible for a cam file to change the behavior of the drill file settings; looks like we have to edit eagle.def for that.
I’m a rookie at eagle, so if there is anyone who knows better, feel free to chime in.
Jake
BTW, I didn't edit my eagle.def file. Jake, did you edit your's? If not, does anyone know why they'd be different?eejake52:
…but it doesn’t appear possible for a cam file to change the behavior of the drill file settings; looks like we have to edit eagle.def for that.
Don
Don> “did you edit yours?”
No, I am using V4.14 and it came with ResX = ResY = 10000. I downloaded a fresh copy of the zip file from cadsoft to check that.
:idea: Just now I checked the release notes for V4.14 and it says:
" Increased resolution of EXCELLON driver to 1/10000 inch."
So the mystery is unraveled!
Sparky,
You should probably update the Eagle FAQ page as follows:
If you are using Eagle V4.14 or later, make a backup copy & edit file eagle.def (in the bin subdirectory), locate the EXCELLON section and change the value of ResX and ResY from 10000 to 1000.
Perhaps a better solution would be to define a new section called EXCELLON_SFE, but that would meant the SFE-Special.cam would need to be changed also.
HTH,
Jake
ok i am emailing this to nathan now, worst thing he wants is 20 or so orders from people with wrong drills (lol)
eejake52:
You should probably update the Eagle FAQ page as follows:If you are using Eagle V4.14 or later, make a backup copy & edit file eagle.def (in the bin subdirectory), locate the EXCELLON section and change the value of ResX and ResY from 10000 to 1000.
weird. i sent in a board a month or so ago made with eagle 4.14 (without any mods to eagle.def) and it came out perfect.
Nall,
On my recent order, SFE corrected the file and sent me an email about it; so my only explanation is that they probably corrected yours too.
If you still have the exact file, please post the first 15 or so lines.
Here is an example of the WRONG format:
%
M48
M72
T01C0.0320
T02C0.0360
T03C0.0440
T04C0.1300
%
T01
X10856Y8792
X10856Y9792
X10856Y11792
X10856Y14792
On the last line, the location of the hole is implied as:
X = 1.0856; Y = 1.4792
SFE wants the file format to show as: X1086Y1479
Jake
Its because they need 2:3 format, with LZ.
So leading zeros can be ommited, BUT there must be 3 decimal places.
eejake52:
Nall,On my recent order, SFE corrected the file and sent me an email about it; so my only explanation is that they probably corrected yours too.
If you still have the exact file, please post the first 15 or so lines.
Well, crap. Here I was feeling good about myself that I hadn’t caused SFE any troubles and my drill files suffered from the same problem you describe:
%
M48
M72
T01C0.0320
T02C0.0400
T03C0.1300
%
T01
X4216Y9992
X4216Y10992
X4116Y13392
X4116Y14392
X6716Y14892
So is the appropriate fix to change eagle.def?
Awesome! Lots of people (undoubtedly myself included) will benefit from this discovery!
Just now I checked the release notes for V4.14 and it says:
" Increased resolution of EXCELLON driver to 1/10000 inch."
Thanks Jake!
Hi - I just got the same message from Ben - but looking at my drd file it seems everything is two 3 decimal places, which I think is what is wanted? I made this in Eagle 4.13, by the way. I followed the instructions here: http://www.sparkfun.com/tutorial/PCB/ea … torial.htm to the word.
%
M48
M72
T01C0.0320
T02C0.0280
T03C0.0400
%
T01
X357Y243
X407Y403
X307Y553
X257Y703
X257Y853
X657Y853
X807Y903
X807Y803
X807Y703
X807Y603
X707Y553
X657Y703
X807Y403
X757Y243
X1107Y403
X1157Y253
X1507Y403
X1557Y253
X1607Y553
X1657Y703
X1657Y853
X1257Y853
X1107Y903
X1107Y803
X1107Y703
X1107Y603
X1207Y553
X1257Y703
X1257Y1033
X1257Y1173
X657Y1173
X657Y1033
T02
X297Y1032
X297Y974
X268Y393
X327Y393
X1588Y393
X1647Y393
X1617Y974
X1617Y1032
T03
X1057Y1203
X957Y1203
X857Y1203
X907Y453
X1007Y453
X957Y253
X1057Y253
X857Y253
M30
I just placed my first PCB order, after reading through the tutorials and this forum. Like NleahciM, I got a reply that next time it would help if my drill file were in 2.3 trailing suppression format.
It seemed to me I had followed the instructions pretty well… As was suggested here, I changed my Eagle.def file so that ResX and ResY in the EXCELLON section are now 1000, whereas previously they were 10,000 (I am using Eagle 4.14).
Here’s the first bit of the drill file I submitted - like NleahciM, it seems to me this is in the correct format. Am I missing something?
LukeZ
%
M48
M72
T01C0.0315
T02C0.0320
T03C0.0400
%
T01
X681Y893
X831Y1343
T02
X1031Y1243
X1131Y1243
X1231Y1243
X1331Y1243
X931Y1143
X931Y1043
X1031Y943
X1131Y943
That looks ok to me. Here’s an excerpt from my SECOND order; this one was accepted with the usual ‘expect delivery in 10 to 18 days’
%
M48
M72
T01C0.0320
T02C0.0440
T03C0.0470
T04C0.0472
T05C0.1102
%
T01
X300Y250
X575Y400
X675Y500
X575Y600
X775Y700
X775Y800
X750Y950
X700Y950
X575Y1100
Jake
Then I suppose the question is, if my drill file really was correct, why the message that next time it would be better if fixed? Given that I’m a relative newbie to this I’m inclined to assume Ben was right and my file was wrong…
Anyways, it would be good to know for sure- it takes an order submission of no errors to get the $2.50 deal in the future, so I’d like to get it right eventually. :?
I just noticed your location. I'm also in Corvallis.LukeZ:
Then I suppose the question is, if my drill file really was correct, why the message that next time it would be better if fixed? Given that I’m a relative newbie to this I’m inclined to assume Ben was right and my file was wrong…Anyways, it would be good to know for sure- it takes an order submission of no errors to get the $2.50 deal in the future, so I’d like to get it right eventually. :?
So we don’t qualify for the $2.50 deal until we get this absolutely perfect? Argh.
By the way - is there any way to check this with Viewmate? I downloaded the program - but I couldn’t figure out how to sue it :o
NleahciM, check out [this thread for a bit of help in using Viewmate. I was able to get it going using that.
Remember that layers in Viewmate don’t correspond to layers in Eagle. All you really need to do is import about 5 Eagle layers, and you can make them layers 1 through 5 in Viewmate if you want. The idea is just to see if they line up. Here’s how I did it (first column is Viewmate layer, second is Eagle file):
Layer 1 - Drill (*.drd)
Layer 2 - Top silk (*.plc)
Layer 3 - Top copper (*.cmp)
Layer 4 - Bottom copper (*.sol)
Layer 5 - Bottom silk (*.pls)
For layers 2 - 5, you can just click on the colored layer box on the left hand side of the Viewmate screen, hit F2, and then select the appropriate Eagle file. For layer 1 however (your drill file), you’ll want to change some settings in Viewmate - Don Blake described this in the thread I posted above, but I’ll reiterate it here: Select layer 1 on the left hand side of the Viewmate window (it doesn’t have to be layer 1 but that’s what we’re using in this example). Go to File->Import->Drill & Rout. The import drill file dialog will appear. Before you import your *.drd file, first click on the Options button at the bottom center of the window. In the drill options that come up, change Left of decimal to 2 and Right of decimal to 3. Then, under the Zeros section, select Omit leading zeros. Click OK to close that box. Now you can select your *.drd file and click Import.
When I first did this my layers looked fine until I did the drill file, and then it all got goobered up. This was before I had changed the EXCELLON section of my Eagle.def file (I’m using Eagle 4.14). After doing that, I reimported everything into Viewmate and it looked good - in some ways you can see what’s going on better than you can in Eagle itself.
LukeZ](http://www.sparkfun.com/cgi-bin/phpbb/viewtopic.php?t=1267)
LukeZ: thanks for the help. I had looked for a topic about viewmate - but somehow I managed to skip over that thread.
Have you figured out yet what is wrong with your drill file? I’d really like to get it figured out as I have a bunch of boards that I’d like to have made…