I appreciate this is a bug report but by using imperial measurements, (For the PCB), instead of metric appears to work just fine for me. All I did was to open your example file in EasyEDA and change the Units to 'inch', exported the gerbers and viewd in Gerbv 2.7.0...  This would suggest it's another imperial / metric conversion, (or lack of), issue. Regards.

@mrtom528, Thanks, that's an excellent bit of detective work. If I get time I'll compare the Gerber files to see if it looks like it is related to the rounding or number formatting which would suggest it is primarily an EasyEDA issue. I have not found any reports from elsewhere that gerbv is misreading drill positions like this, which I would expect to find since I believe gerbv is still the viewer used in Kicad as well as gEDA so there's a sizeable user base.

@andyfierman No worries. As to checking the files.....this has already been addressed in post [Incorrect Drill Holes](https://easyeda.com/forum/topic/Incorrect-Drill-Holes-Position-0cd73ab552834d8ca510da0e94898d51) which highlights that the formatting of metric X & Y values is incorrect to the tune of an additional zero. Editing your [metric] drill file X & Y values by deleting the leading zero cures the problem.....so I guess it's an EasyEDA error when writing the values to gerber files. Regards.

@mrtom528, Yes, I'd linked my Bug Report to [Incorrect Drill Holes](https://easyeda.com/forum/topic/Incorrect-Drill-Holes-Position-0cd73ab552834d8ca510da0e94898d51) but your simple little sanity check pretty much proves that it's the same EasyEDA issue, just that it shows up in some gerber viewers and not others. Many thanks again. :)

@andyfierman, No worries.....but here's a strange thing... _ Instead of saving the gerber files out to a zip file I tried directly ordering from JLCPCB...so...Fabrication > Generate PCB Fabrication File (Gerber) > Order at JLCPCB (Blue button bottom right of window) > OK (At prompt) _ This auto uploads and opens the Gerber files for viewing which, to me, look absolutely fine. Clicking the 'Gerber Viewer' link bottom right of the preview also shows no error in the drill position, in fact this can toggled on or off and clearly shows it to be correct. _ So are the files correct or not? Will we ever get to the bottom of it? Will it snow again this year? Tune in next week for another thrilling episode of 'The Gerber-Files'. _ Regards.

I can't  wait! Can't I ust get the whole series to binge read? :)

That seems Gerbv 2.7.0 doesn't match the Gerber unit, after checking at Gerbv 2.6A it works well. It looks same as flatCAM issue Eric: `flatcam` cannot recognize `0000.00` format drill files. It only works with `000.000` format. I tested some other softwares like `GerbView, Gerbv, ViewMate`, they works fine. `EasyEDA` may should export drill files as `000.000` format by default. The limitation of `000.000` format is that the big boards longer than 1 meter cannot be present, except you use `INCH` unit instead of `METRIC`. A few users need such big size boards.

After checking, Gerbv 2.7.0 has a different detection for the Drill format  You can change the digits of drill file.

Gerbv 2.6 works well, but  Gerbv 2.7 has problem. You can manual setting number format. 1\. Select your drill file layer 2\. Menu \-\> Layer \-\> Edit file format\, see a setting dialog 3\. Set as: NOT autodetect\,  Leading\, mm\, 2 digits 4\. Click OK   

@eric, @UserSupport, Thanks! I did not know about that setting. I will check it and edit this Bug Report.

Hi! So, you guys say that is it preferrable to generate gerbers in inches mode? At least I have always generated in inches mode and I haven't had any these kind of problems. Regards, Markus Virtanen HW / Electronics Designer

@markus_jidoka, For the moment it looks like it's safer to generate Gerbers in inches or mils. Beware however that switching units may then generate DRC errors in the PCB Editor due to rounding errors. Perhaps the way to do this is to do the final DRC in whichever units the PCB has been designed in and then, if required, switch to inches/mils and generate the Gerbers.

@markus_jidoka, Just my findings so far: Further investigation shows that using the Desktop Client (6.4.7) works just fine regardless of using metric or imperial measurements. The online version fails for metric units when using a gerber **viewer** but is fine for uploading gerber files to JLCPCB, either directly or in zip format. _ The simple difference between the two is the format of coordinates in the .DRL files, the Desktop Client uses X+012500Y+012500, whilst the Online uses X001250Y001250. It therefore appears that a simple change in the format by replacing the leading zero with a sign (+/-) would work. _ I've tested this by manually editing the Online created .DRL file as described above and It works just as the Desktop Client, without errors. _ Lets hope it's fixed for the 6.4.14 version of the Desktop Client.....or will it be 6.4.12....????? _ Regards.

@mrtom528 It should be fixed by JLCPCB, EasyEDA Gerber format is matching the Gerber rule.

`This seems to be another example of where the drill holes end up in the wrong place: `<br> <br> [https://easyeda.com/forum/topic/Gerber-drill-layer-small-and-out-of-place-6437a04009f94682a070a156b401b009](https://easyeda.com/forum/topic/Gerber-drill-layer-small-and-out-of-place-6437a04009f94682a070a156b401b009)