Does anybody know of a freeware (or pay) program that will generate Excellon .DRL files from Gerbers? My CircuitMaker2000 is finally giving up the ghost and refuses to do the job - the .DRL files is coming out with no drill hole sizes. I’m in the process of moving across to kiCAD 6, but it’s a steep learning curve and I don’t want to have to redesign the board as a first project at this stage.
Andrew, isn't the drill file part of a Gerber set? Are you saying that that file is missing from the CM2000 Gerber output?
Jan
Jan
KiCAD 6 vs KiCAD 7 is not that different. I do agree that you should be using the latest version, though. Most importantly: Don't bother learning KiCAD 5 as the change from 5 to 6 was significant.
Gerber files don't contain any drill information. The drill (X,Y) and diameter are in the Echelon drill file. It's just a text file. You should be able to edit it in any text editor (Notepad, vi, textedit, etc.) and make it work that way. Then verify with a Gerber viewer that you have it right. I personally like https://www.gerber-viewer.com/
Once you have all the fabrication outputs you might be able to import the board into KiCAD. I'm not sure why you would, though. Unless it's a super complicated or large board it's probably better to just redraw it if you want to edit it. And if you don't want to edit it you don't need to import anything.
Tom
Gerber files don't contain any drill information. The drill (X,Y) and diameter are in the Echelon drill file. It's just a text file. You should be able to edit it in any text editor (Notepad, vi, textedit, etc.) and make it work that way. Then verify with a Gerber viewer that you have it right. I personally like https://www.gerber-viewer.com/
Once you have all the fabrication outputs you might be able to import the board into KiCAD. I'm not sure why you would, though. Unless it's a super complicated or large board it's probably better to just redraw it if you want to edit it. And if you don't want to edit it you don't need to import anything.
Tom
This might make manual editing of Echelon files easier: https://www.artwork.com/gerber/drl2laser/excellon/index.htm
Tom
Tom
Jan, yes I think so. I sent the files off for manufacture and the .DRL file is in the set of outputs, but it’s coming up empty ie all the hole sizes are showing zero. The file generation is the same as I’ve always used so I’m suspecting it’s because Windows has updated and/or I have a new PC. I do now need to transition to kiCAD so this will be my last Circuit2000 board.
Thanks Tom - I did have kiCAD 5 but never transitioned so I downloaded 6 yesterday (with a donation) and that what I’ll move forward with.
The PCB in question has a few hundred holes so not really conducive to a manual edit.
Maybe an SMD version is in order then... 😉
OK, so seriously: You may have hundreds of holes but you probably only use 4-5 different hole diameters. If not, you can probably reduce the drill count. As far as I understand it, the Echelon file defines the tools (i.e., the drill diameters) early in the file and then lists "Tool 1, X, Y, RPM" etc. So it should only be the tool definitions that you need to edit. So you'll need to make five edits for five drill diameters. That seems manageable.
Tom
Hi Andrew,
Well that’s a surprise and a pita to go with it. How about using a different pc with windows 7 to run your circuitmarker sw? Until you get up to speed on kicad.
It’s a lot of work to manually create a excellon drill file from Gerber data. You can figure out the drill hit locations by determining the pad/flash centroid but figuring out the drill size is not so obvious from the Gerber data. You would need to determine the pad stack drill size that was used to create pad in the Gerber file or know the lead diameter that is used to fit the hole and add the necessary clearance.
Well that’s a surprise and a pita to go with it. How about using a different pc with windows 7 to run your circuitmarker sw? Until you get up to speed on kicad.
It’s a lot of work to manually create a excellon drill file from Gerber data. You can figure out the drill hit locations by determining the pad/flash centroid but figuring out the drill size is not so obvious from the Gerber data. You would need to determine the pad stack drill size that was used to create pad in the Gerber file or know the lead diameter that is used to fit the hole and add the necessary clearance.
Last edited:
KiCad 6 has been out of support since December 2022, so getting stale. I don't advise trying 7.99 now and 8.0.0 when it comes out very soon, as the first month or two of a new release can get messy. Also the tutorials out there won't have caught up.
In KiCad there is an option to generate the Excellon files when you create the Gerber set, Excellon is NOT Gerber.
An alternative might also be to install an older OS in a virtual machine and run your CAD program there. There's no logical reason why the software should suddenly have stopped working unless it relies on dot-net or something and Microsoft broke something in an update.
Virtualbox can be helpful: https://www.virtualbox.org/
Tom
Virtualbox can be helpful: https://www.virtualbox.org/
Tom
It sounds like you are experiencing the same issue I ran into when using an old version of Eagle PCB software. Your software hasn't changed, but the file format the PCB house expects has. Here is a copy of a note I keep on my desktop on how to fix the file.
Version 4.1 of EAGLE generates an older version of the EXCELLON drill file (.XLN)
The old version requires a drill file (.drl) to define the drill sizes.
The new version that JLCPCB wants imbeds the drills in the EXCELLON file.
The drill (drl) file would look like this:
T01 0.024in
T02 0.040in
T03 0.079in
T04 0.100in
So use this info to add these lines to the .XLN file:
T01C00.024
T02C00.040
T03C00.079
T04C00.100
as shown below:
In inches:
%
M48
M72
T01C00.024
T02C00.040
T03C00.079
T04C00.100
T01
X519Y442
X485Y741
X789Y791
X1035Y895
X680Y1001
X523Y962
X1271Y608
X1615Y149
X1066Y139
T02
X1486Y387
X1486Y487
X1486Y587
X1486Y687
X1486Y787
T03
X1705Y773
X1705Y502
X190Y588
X190Y938
T04
X562Y1090
X1350Y165
M30
you can use the export function in gerv.exe to correct the formatting:
M48
INCH,TZ
T10C0.024
T11C0.040
T12C0.079
T13C0.100
%
T10
X000519Y000442
X000485Y000741
X000789Y000791
X001035Y000895
X000680Y001001
X000523Y000962
X001271Y000608
X001615Y000149
X001066Y000139
T11
X001486Y000387
X001486Y000487
X001486Y000587
X001486Y000687
X001486Y000787
T12
X001705Y000773
X001705Y000502
X000190Y000588
X000190Y000938
T13
X000562Y001090
X001350Y000165
M30
WITH METRIC EXCELLON:
%
M48
M71
T01C00.61
T02C01.02
T03C02.01
T04C02.54
T01
X1318Y1123
X1233Y1883
X2003Y2008
X2628Y2273
X1728Y2543
X1328Y2443
X3228Y1543
X4103Y378
X2708Y353
T02
X3774Y983
X3774Y1237
X3774Y1491
X3774Y1745
X3774Y1999
T03
X4330Y1964
X4330Y1275
X482Y1494
X482Y2383
T04
X1428Y2768
X3428Y418
M30
Hope this helps,
Terry
Version 4.1 of EAGLE generates an older version of the EXCELLON drill file (.XLN)
The old version requires a drill file (.drl) to define the drill sizes.
The new version that JLCPCB wants imbeds the drills in the EXCELLON file.
The drill (drl) file would look like this:
T01 0.024in
T02 0.040in
T03 0.079in
T04 0.100in
So use this info to add these lines to the .XLN file:
T01C00.024
T02C00.040
T03C00.079
T04C00.100
as shown below:
In inches:
%
M48
M72
T01C00.024
T02C00.040
T03C00.079
T04C00.100
T01
X519Y442
X485Y741
X789Y791
X1035Y895
X680Y1001
X523Y962
X1271Y608
X1615Y149
X1066Y139
T02
X1486Y387
X1486Y487
X1486Y587
X1486Y687
X1486Y787
T03
X1705Y773
X1705Y502
X190Y588
X190Y938
T04
X562Y1090
X1350Y165
M30
you can use the export function in gerv.exe to correct the formatting:
M48
INCH,TZ
T10C0.024
T11C0.040
T12C0.079
T13C0.100
%
T10
X000519Y000442
X000485Y000741
X000789Y000791
X001035Y000895
X000680Y001001
X000523Y000962
X001271Y000608
X001615Y000149
X001066Y000139
T11
X001486Y000387
X001486Y000487
X001486Y000587
X001486Y000687
X001486Y000787
T12
X001705Y000773
X001705Y000502
X000190Y000588
X000190Y000938
T13
X000562Y001090
X001350Y000165
M30
WITH METRIC EXCELLON:
%
M48
M71
T01C00.61
T02C01.02
T03C02.01
T04C02.54
T01
X1318Y1123
X1233Y1883
X2003Y2008
X2628Y2273
X1728Y2543
X1328Y2443
X3228Y1543
X4103Y378
X2708Y353
T02
X3774Y983
X3774Y1237
X3774Y1491
X3774Y1745
X3774Y1999
T03
X4330Y1964
X4330Y1275
X482Y1494
X482Y2383
T04
X1428Y2768
X3428Y418
M30
Hope this helps,
Terry
I still have my older PC. I am going to copy the file onto that and see what happens.
Separately, If I am going down the kiCAD route, what version is recommended? (I noted on V5 that there did not appear to be any packages for power transistors and the transistor selection was quite limited. In CircuitMaker2000, you just use a transistor symbol, then attach a package to that and a device name (eg MJE15033) and a part number (e.g. Mouser 555-45613).
I guess I will have to think in a new way to get a grip of this.
Separately, If I am going down the kiCAD route, what version is recommended? (I noted on V5 that there did not appear to be any packages for power transistors and the transistor selection was quite limited. In CircuitMaker2000, you just use a transistor symbol, then attach a package to that and a device name (eg MJE15033) and a part number (e.g. Mouser 555-45613).
I guess I will have to think in a new way to get a grip of this.
I came from an ancient version of OrCAD. There's definitely a learning curve with KiCAD, but I didn't find it overwhelming. It's not like Altium where it took me an hour to figure out that there are multiple ways of opening the same file and they all produce different results.
Beware that KiCAD has presets for touchpad and mouse in the editor. Make sure you have the correct one selected. I also change the coordinate system in the PCB layout editor from quadrant IV (positive X, negative Y coordinates) to quadrant I (positive X and Y).
Watch a couple of Intro to KiCAD videos. I bet you'll get a hang of it within a day.
Tom
Beware that KiCAD has presets for touchpad and mouse in the editor. Make sure you have the correct one selected. I also change the coordinate system in the PCB layout editor from quadrant IV (positive X, negative Y coordinates) to quadrant I (positive X and Y).
Watch a couple of Intro to KiCAD videos. I bet you'll get a hang of it within a day.
Tom
Andrew,
I investigated Circuitmaker, it's a free pcb toolset?
is it some version of ? https://www.altium.com/circuitmaker
So I assume it is an Altium database, which one could BUY a current toolset 🙂
Justification is favourable, if one has a business to support a development tool expense 🙂
How many cases of the finest wine is it ?
A current version of Altium would save your IP, preserve old designs, libraries etc, it is a path forward
I see there is Circuit Studio and full flegged Altium, do not know the $ however.
If your pcbs can be designed on free s/w they can't be that complicated 🙂
One time we were designing pcbs using Cadence Allegro, the dev Lab was sold to HP,
you're now going to be using Mentor Graphics Board Station500, off to class in San Jose,
for a week, met some nice ladies from the HP McMinville CAD group ... fun times 🙂
bunch of rats jumping ship
I have a similar issue in still using Orcad16 ... but I have a path forward using Cadence and ponying up some $
or go the Kicad route as you are investigating.
I have a huge investment of my time into custom libraries.
I investigated Circuitmaker, it's a free pcb toolset?
is it some version of ? https://www.altium.com/circuitmaker
So I assume it is an Altium database, which one could BUY a current toolset 🙂
Justification is favourable, if one has a business to support a development tool expense 🙂
How many cases of the finest wine is it ?
A current version of Altium would save your IP, preserve old designs, libraries etc, it is a path forward
I see there is Circuit Studio and full flegged Altium, do not know the $ however.
If your pcbs can be designed on free s/w they can't be that complicated 🙂
One time we were designing pcbs using Cadence Allegro, the dev Lab was sold to HP,
you're now going to be using Mentor Graphics Board Station500, off to class in San Jose,
for a week, met some nice ladies from the HP McMinville CAD group ... fun times 🙂
bunch of rats jumping ship
I have a similar issue in still using Orcad16 ... but I have a path forward using Cadence and ponying up some $
or go the Kicad route as you are investigating.
I have a huge investment of my time into custom libraries.
Last edited: