Skip to main content ↑ ↓
Topic: Checking drill file accuracy (Read 2332 times) previous topic - next topic

Checking drill file accuracy

I just got my first order.  Expedited + DHL China got me 7 day turnaround!  Unfortunately there are a number of problems with the drill holes on the board.  Some footprints are missing holes altogether and others are larger than I expected.  In particular the mounting holes which were supposed to be a #4 clearnace hole with a large pad, but came out with a large hole and almost no pad.  I checked the gerbers with a gerber viewer, but of course that doesn't show the drill holes.

Can anyone suggest a way to check the accuracy of the drill file before sending off a job?

Re: Checking drill file accuracy

Reply #1 –
you can view the drill file (*.TXT) together with the other gerber files.

Re: Checking drill file accuracy

Reply #2 –
I figured out what I did wrong.  I included the .drl file, but not the .TXT file in the zip.  Do you know of a gerber viewer that can show the .TXT file for visual verification?

Re: Checking drill file accuracy

Reply #3 –
There are plenty of online viewers which should be able to show the drills. Here's one (not saying it's the best, but I've used it before): http://gerblook.org/

You can also try uploading it to the OSHPark site without ordering the PCB, they have a nice built in viewer (but I think you need to make an account).

In Kicad, I only get one drill file which is labeld ".drl". I then use a python script to rename the ".drl" to ".txt" so it's recognized by most of the online PCB services. I'm not quite sure why you have two drill files (you have both a ".drl" and a ".txt")? Maybe it's used for some advanced thing I don't know about (like separate mounting hole/plated hole files)...

Re: Checking drill file accuracy

Reply #4 –
I found that Gerbv can load the .TXT file, but not the .dri file.  It shows tiny spots where the holes should be, presumably because the hole sizes are called out in the .drl file.  Also, I have to scale that layer by 0.1 to get it to match the board.  Anyone know if that's going to be a problem for the board house?

Re: Checking drill file accuracy

Reply #5 –
What program are you using to make the PCB? Maybe you can change it in the export options/someone else who uses the program can tell you how to fix it?

Re: Checking drill file accuracy

Reply #6 –
gerbv has no issues with loading an Excellon drill file with a .drl extension, it should show exactly the holes, at the correct size, without any manual scaling, anything you have to do like that indicates a problem in your files.

I would say then, that your .drl file is not in fact an Excellon drill file, which is the type of file that is required.

If you are making a simple 2 layer board with only plated holes (no unplated holes, I don't know if they are even supported by Dirty), then you should only be providing the single Excellon drill file - with a .txt file extension, and the other gerber layer files (gt[lso], gb[lso] and gko for the outline).

The extension is just that, a file extension that allows the board house to recognise what layer is what, converting an Excellon drill file with a ".drl" extension to a ".txt" file is exactly renaming the file.

If you posted your gerbers zipped up it might make it clearer.  And specify which software you generated them from.

Re: Checking drill file accuracy

Reply #7 –
Also, maybe you are using Eagle, in which case...
http://electronics.stackexchange.com/qu ... ro-suppres
http://forum.sunstone.com/eagle-softwar ... e-t18.html

I don't use Eagle, but others do and would be able to guide you on how to properly export a working drill file.

In short, if the holes don't look right in gerbv without fiddling, something is screwy and you will probably get screwy boards.

Re: Checking drill file accuracy

Reply #8 –
Good pointers, thanks.  To summarize for anyone else having this issue, the .TXT file has all the needed drill information and the .dri file can be ignored.  Newer versions of Eagle (7.2 and higher) use a high resolution excellon format that confuses Gerbv and may also confuse the board house.  You can fix that by specifying the CAM job to use the EXCELLON_24 format rather than just EXCELLON.  My gerbers look great in Gerbv now and the drill file shows holes the correct size and location.