Drill file format

[deephaven]

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-1842T1
X2734Y-1637
X5687Y-1766
X2305Y-1647
X4571Y-3302
X4571Y-2004
X4530Y-3541
X4919Y-3153
X3180Y-3705
X1990Y-3310T2
X1990Y-3110
X1990Y-2910
X1990Y-2710
X1990Y-2510
X2141Y-1173T3
X2014Y-1427
X1887Y-1173
X1760Y-1427
X3904Y-508
M30


The 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?

[jahonen]

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:

M48
METRIC,TZ
%
T1C1.02
X192785Y222665
X232915Y222665
X232915Y241335
T2C1.1
X306340Y186000
X306340Y191080
X306340Y188540
T3C2.1
X105200Y113800
X105200Y161000
X105200Y179300

Regards,
Janne

[deephaven]

Thanks for the useful comments and example Janne.

[Rufus]

(Poor) documentation on the Excellon drill file format is here http://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.

[Rufus]

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. 

[deephaven]

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. 

Thanks 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.

[Rufus]

Thanks 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

I 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.

[C_Ehlen9999]

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

[Feynman]

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

EAGLE would be my guess.

[Doctorandus_P]

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.

My 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.