Problems with excellon NC drill output

[Anders Nelson]

To whoever can help me-->

I am a user of EAGLE light and I am getting crazy excellon file output.
I go through PCBExpress.com's drillcfg.ulp to setup the tool sizes, then
EAGLE's excellon.cam job, then PCBExpress.com's E1.cam. I always get the
proper Gerber files, but my drill file (.drd) puts holes all over the
place, all teh same size. I am previewing my Gerber files through
Viewmate by Pentalogix.

Anyone have any ideas? Thanks!

[Tilmann Reh]

Post by Anders Nelson
I am a user of EAGLE light and I am getting crazy excellon file output.
I go through PCBExpress.com's drillcfg.ulp to setup the tool sizes, then
EAGLE's excellon.cam job, then PCBExpress.com's E1.cam. I always get the
proper Gerber files, but my drill file (.drd) puts holes all over the
place, all teh same size. I am previewing my Gerber files through
Viewmate by Pentalogix.

We've heard about problems with Viemate many times. Try GCprevue instead.

Also, take care that there are different usual drill data formats, in
terms of the number of decimals. If you're off by one digit, all drill
data is scaled by a factor of 10 (or 0.1) in your viewer. The board
houses usually detect the format correctly and make good boards, though. :-)

[James Morrison]

Post by Tilmann Reh

Post by Anders Nelson
I am a user of EAGLE light and I am getting crazy excellon file output.
I go through PCBExpress.com's drillcfg.ulp to setup the tool sizes, then
EAGLE's excellon.cam job, then PCBExpress.com's E1.cam. I always get the
proper Gerber files, but my drill file (.drd) puts holes all over the
place, all teh same size. I am previewing my Gerber files through
Viewmate by Pentalogix.

We've heard about problems with Viemate many times. Try GCprevue instead.
Also, take care that there are different usual drill data formats, in
terms of the number of decimals. If you're off by one digit, all drill
data is scaled by a factor of 10 (or 0.1) in your viewer. The board
houses usually detect the format correctly and make good boards, though. :-)

This is almost for sure an issue with 2.3 vs 2.4 format of drill
locations. As Tilman says, getting it wrong gives a scale error of 10x.

To tell what Eagle is generating go to $EAGLEBIN and open the file
called eagle.def. Search in there for the section called Excellon.

If the line RESX and RESY are set to 1000 then you are generating 2.3
format. If they are 10000 then you are generating 2.4. There is a
setting in the advanced options of Viewmate import ncdrill to set the
format.

BTW, I noticed that version 4.15 changed from default 2.3 to default
2.4. The only reason I noticed is because on a board pre-4.15 that was
very small and dense the PCB manufacturer complained because there
appeared to be a "small random offset" in the drill locations with
respect to the pads and with an annular ring of 0.004" it made a
difference. The problem was the rounding error of the 2.3 format. I
went and changed to 2.4 explicitly and they were much happier.

Cheers,

James.

[Anders Nelson]

GCPrevue works perfectly! Thanks!

Post by Tilmann Reh
We've heard about problems with Viemate many times. Try GCprevue instead.
Also, take care that there are different usual drill data formats, in
terms of the number of decimals. If you're off by one digit, all drill
data is scaled by a factor of 10 (or 0.1) in your viewer. The board
houses usually detect the format correctly and make good boards, though. :-)