Drill file format - Page 1
Forum section: electronics / general

author: deephaven
author_rank: Frequent Contributor
timestamp: June 02, 2011, 08:33:32 am
content: I've never had a problem with PCB companies interpreting my submitted drill file correctly and producing PCBs with holes in the correct places. Until Now. I thought I would try iTead Studio and was really pleased with the quality of the boards, how quickly they got delivered to me and the cost. However, I noticed that just two of the holes were the incorrect size. I reported it back to them and they came back and said there was an error in my file. Here is a cut-down version of it's contents:%X2876Y-1842T1X2734Y-1637X5687Y-1766X2305Y-1647X4571Y-3302X4571Y-2004X4530Y-3541X4919Y-3153X3180Y-3705X1990Y-3310T2X1990Y-3110X1990Y-2910X1990Y-2710X1990Y-2510X2141Y-1173T3X2014Y-1427X1887Y-1173X1760Y-1427X3904Y-508M30The problem is due to the placing of the T1 etc and I can understand what they mean. I had always assumed that it was correct as that is what my CAD programme outputs and it has never been a problem before. Could someone comment on what should be the correct format if this is wrong? I assume T1 should occur before any XY values - and on it's own line?

author: jahonen
author_rank: Super Contributor
timestamp: June 02, 2011, 09:24:16 am
content: I think that tool change commands(?) lines should be on their separate lines like you suspect. Also, you seem to have negative coordinates in the drill file, which is thing to avoid also (check alignment with gerber coordinates, although CAM operator can align layers, it is better to ensure this before sending out files). Furthermore, I think it would be also wise to include drill sizes, so the file should probably look something like this:M48METRIC,TZ%T1C1.02X192785Y222665X232915Y222665X232915Y241335T2C1.1X306340Y186000X306340Y191080X306340Y188540T3C2.1X105200Y113800X105200Y161000X105200Y179300Regards,Janne

author: deephaven
author_rank: Frequent Contributor
timestamp: June 02, 2011, 11:44:15 am
content: Thanks for the useful comments and example Janne.

author: Rufus
author_rank: Super Contributor
timestamp: June 02, 2011, 04:24:53 pm
content: (Poor) documentation on the Excellon drill file format is herehttp://www.excellon.com/manuals/program.htm.Apart from in some repeat commands it doesn't say that new lines or white space are significant or required. It sort of implies that each hole command and tool change will be on a separate line.I would say that whatever generated that drill file with tool changes tacked on the end of drill lines is poor just from a readability point of view. Whatever read it and apparently ignored parts it didn't understand without complaint is worse.

author: Rufus
author_rank: Super Contributor
timestamp: June 02, 2011, 08:59:33 pm
content: In passing I spoke to someone more knowledgeable about this and drill files with tool changes on the end of a line are in Sieb Meyer format.The file starting with a %%1000 or %%3000 is also an indication of Sieb Meyer format.In Sieb Meyer tool changes are always on the end of a line and apply to the hole on that line and subsequent holes.In Excellon it is debatable if a tool change on the end of a line is valid at all. It seems iTead accepted it or mistakenly corrected it and applied it to subsequent holes.Sieb Meyer is much less common than Excellon, surprised you have a package that generates it at all, or apparently by default.

author: deephaven
author_rank: Frequent Contributor
timestamp: June 02, 2011, 09:09:21 pm
content: Quote from: Rufus on June 02, 2011, 08:59:33 pmThanks for the info, Rufus. I use a German CAD package which may explain why it defaults to Sieb Meyer, well it sounds German! It's never been an issue before, so it's not something I've looked into before. I can set the output to Excellon format, however, when I try to load it into GCPrevue, the scale is wrong. I played around with the number of significant digits and inches/mm but can't get it to load with the same scale as the Gerber files. I must admit to working in the dark a bit and I need to read up more on the significance of the settings. I can manually edit the Sieb Meyer file, but it would be nice to come up with a solution which is inherently right.

author: Rufus
author_rank: Super Contributor
timestamp: June 03, 2011, 12:08:44 am
content: Quote from: deephaven on June 02, 2011, 09:09:21 pmI guess whoever did your boards before recognised it as Sieb Meyer and either worked with it or converted it correctly.It is strange the formats are similar enough to be confusing, they diverge more when it comes to routing commands.

author: C_Ehlen9999
author_rank: Newbie
timestamp: July 25, 2023, 10:17:26 am
content: Hi Deephaven,Sorry to revisit this after 12 years, but as it happens I require software that exports in Sieb & Meyer format for our CNC. As Rufus suggested, it's very difficult to come by such a software. Could you please let me know which software it is that you were using then?Many thanks,Chris

author: Feynman
author_rank: Regular Contributor
timestamp: July 26, 2023, 04:08:50 pm
content: Quote from: C_Ehlen9999 on July 25, 2023, 10:17:26 amEAGLE would be my guess.

author: Doctorandus_P
author_rank: Super Contributor
timestamp: September 11, 2023, 10:07:18 am
content: Quote from: C_Ehlen9999 on July 25, 2023, 10:17:26 amMy first thought was to replace the (very likely obsolete) controller of your CNC machine. You can for example use LinuxCNC.Second thought is to either get a file converter or write it yourself. It's quite simple text manipulation.