Using GerbView to import Proteus drill file

[741]

I am converting a set of Gerbers generated by Proteus to Kicad. I have only the Gerbers & drill file.

The gerbers imported fine. A README file indicates “CADCAM Drill TOP-BOT Plated.GBR” is the drill file.

So I re-named the file - but the drill import failed

The file starts like this -

04 PROTEUS GERBER X2 FILE
%TF.GenerationSoftware,Labcenter,Proteus,8.9-SP0-Build27865*%
%TF.CreationDate,2020-10-20T16:57:33+00:00*%
%TF.FileFunction,Plated,1,2,PTH*%
%TF.FilePolarity,Positive*%
%TF.Part,Single*%
%TF.SameCoordinates,{76c10f42-4764-4ffd-9dd0-b871e5010a22}%
%FSLAX45Y45%
%MOMM*%
01
%TA.AperFunction,ViaDrill*%
%ADD123C,0.500000*%
%ADD124C,0.350000*%
%ADD125C,0.250000*%
%TA.AperFunction,ComponentDrill*%
%ADD126C,1.500000*%
%TA.AperFunction,ComponentDrill*%
%ADD127C,0.965200*%
%TA.AperFunction,ComponentDrill*%
%ADD128C,0.762000*%
%TD.AperFunction*%
123
+8610000Y+3899000D03
+8360000Y+3949000D03
+9180000Y+3949000D03
+9396920Y+3950000D03
124

The other thing is that when I choode “export to PCBNEW” all pads (SMD and PTH) are round and the pattern at the front is copied to the back.

[paulvdh]

@741

I have only the Gerbers & drill file.

Do you have the schematic?

I have done a few experiments in this direction and generally don’t bother with drill files.

The whole concept of “footprints” hardly exists in the gerber files, and therefore I do not even try to reconstruct it, because it’s very easy to simply use new footprints.
So I just throw away all the re-imported pads, then recreating the schematic and position new footprints over the ends of the existing tracks.

I did a write up about that (which still needs cleanup) and posted it:

Reverse engineering KiCad project from Gerber files

2021-09-06Txx:xx Work in Progress. Incomplete! 2021-09-06T15:15 It’s fairly complete now. Time for something completely different. Some help with proofreading and finding missing or unclear parts is appreciated. The goal of this reverse-engineering tutorial is to re-create a complete KiCad project from partial information. I assume the only information available is a schematic in some readable, (but not EDA form, such as a .pdf or a .png picture, and a set of gerber files. In short, the step…

[741]

Thanks! Immediate improvement after reading just some of your guide. I’ll keep reading…

[Frederik]

The file you list is in Gerber format, and you seem to read it with an Excellon NC format input.
Apart from that, there are some strange lines in the Gerber file, like
04 PROTEUS GERBER X2 FILE
Could it be that you copied it wrong, and it is actually?
G04 PROTEUS GERBER X2 FILE
You could check the file on the Reference Gerber Viewer, that should be able to tell you whether it is valid Gerber or not.

[741]

OK - Thank you.

Because the README file showed that “CADCAM Drill TOP-BOT Plated.GBR” was the “drill” file, I re-named it to “CADCAM Drill TOP-BOT Plated.DRL”…

Now I have restored the “.GBR” extension - and it loads

Question: Why is it that we need “Excellon Drill Files” if the Gerber format supports drilling data?

[eelik]

@741

Question: Why is it that we need “Excellon Drill Files” if the Gerber format supports drilling data?

Because Excellon has been used for so long and many manufacturers expect it or at least understand it, and some may not handle Gerber drill files directly.

That’s the basic problem with everything related to Gerber. Even though it is about as good and modern file format than other formats, it has too much historical baggage. Recommendations and best practices can’t be forced for output (EDA software) or input (manufacturers/CAM software), and especially cheap and popular manufacturers use old software and old conventions, and even so that different manufacturers use different conventions. I would like to see even one cheap manufacturer who actually takes modern Gerbers with all recommended and best practices so that everything possible in a design is defined in the Gerber files and nothing else is needed.

[Frederik]

It is indeed said that some fabricators do not handle Gerber drill files. However, I wonder if this is still true, or, rather, to what degree it is not true. Thinks slowly, very slowly, improve.
Does one know fabricators that would refuse a job because the drills are in Gerber?