genrate drill file from gerber and fab data

No, you will have to get your pcb fabricator to make a drill file for you...sounds expensive...

OR........ can you import the gerber layers into your pcb package, then place vias over every pad/hole and make a drill file from that?

This demonstrates why specialized tools exist what a bad idea it is to use the wrong tool for the job.

Another element you are missing in your inappropriate tool:

The depths to which I despise Autocad for PCB's knows no bounds. I still occasionally run into people with .dxf or .dwg's, but it's becoming very infrequent now. However, the short answer is yes you can generate a drill file by hand. Import to Viewmate (freeware) to verify.

Below is a sample drill file from one of my small boards. Use the following link to help interpret

Notice that each line only shows the coordinates which changed. T1-T4 in the beginning defines the drill diameters in inches. Not sure what the M72 & M48 commands are. Assuming M30 means stop...

Happy hunting!

Chris

--------

M72 M48 T1F00S00C0.0200 T2F00S00C0.0460 T3F00S00C0.0520 T4F00S00C0.1500 % T01 X014100Y014750 Y018900 X017100Y018350 X019000 X018000Y031000 Y031500 X017500 X017000 X016500 X016000 Y031000 X016500 X017000 X017500 T02 X005300Y010000 X007300 X009300 X003300 X002250Y015500 Y017500 Y019500 X003300Y025000 X005300 X007300 X009300 T03 X023600Y015450 X026300 X026050Y029450 X022800Y029440 T04 X034900Y005000 X016500 X032800Y022100 M30

I do not know what you mean by "..all the other Gerber files..." - other to what? The Apertures file is a simple ascii file: as to why you have more than one for your pcb I am bemused. The Gerber files contain all the layout data for the pcb - thats why Gerbers are used (so that the pcb house does not have to keep copies of every single piece of drafting sotware yet invented).

If you do have the Gerbers (it will be a type 274D if it requires a seperate apertures file) just dowload a free Gerber viewer -there are many so try Viewmate, GC Prevue or whatever takes your fancy as they will all help you - and you will be able to see the pcb. Wade through the helpfile and learn what to do. You will have to do some work such as identifying and / or sizing the holes.

Many pcb design packages have a gerber import facility to allow you to dothe same.

You are obviously not familiar with pcb design so please note that there is no universal standard for the naming of file types in the pcb world. A dot.pcb file is just the name chosen by that particular software company - I know of three different formats/file types called dot.pcb and I am sure there are others. Ditto with names used for Gerbers but the gerber files themselves are in a universally standard format/file type.

Good luck

VK, There is no easy or simple manner for anyone to describe to you how to rebuild/regenerate a drill file for your files. It can be done, it can be done fairly easily by someone that fully understands what they are doing and have access to a suitable Gerber editing tool. The key there is a Gerber tool that will do file editing, typically any of the freely available tools on the internet are just Gerber viewers. If this was a medium size/complexity board with mostly SMT components, a few mounting holes and a bunch of vias, I don't see why I wouldn't be able to manually ressurrect the drill data in an hour or two, but then I have been doing PCB design for decades. However I could spend three - four times that amount of time just trying to explain to you what you need to do and how to do it.

So far I have only seen one suitable answer to your enquiry from other posters, seems most of them don't know how to read your original post and they are looking for a reason to rant about AutoCAD or the precise formatting of the Gerbers you have obviously inheritted from someone else. Don't worry, having a fabrication drawing done in AutoCAD is very common, I have done it that way for decades because ECAD/PCB CAD tools typically suck big-time as a general drawing or documentaion tool.

(Note: the original post said nothing other than he had a "fabrication drawing" in AutoCAD format, not a PCB design, nor Gerbers generated from an AutoCAD PCB design.)

There is one slight possiblity that could be your saving grace. Do you have a Gerber viewer and have you loaded and viewed the Gerber files? Is there a Gerber file that appears to be only the holes for the board? This would be strictly circular flashes on a layer all by themselves, no traces or other lines, except maybe a board outline, titleblock or drawing template surrounding the board itself. These flashes are they sized appropriately for the desired hole sizes (query them with your viewer tool and it should tell you the aperture (flash) size, this should match to the drill sizes called out in the fabrciation drawing if it contains the drill sizes). If you have one of those layers in your Gerbers, almost any fabrciator can turn that Gerber layer into a drill file in minutes and your problem is solved.

If you desire, you could send me the files in question and I could give them a looking over your you and then be in a position better advise/assist you.

bveland at shaw dot ca

If you have the gerber files, you should be able to set a flag in the setup routine in ORCAD to generate the drill file. There are some other tools that can generate drill files from Gerber files that do not require PCB layout. However, if you have a precision AUTOCAD file this might also work. If all else fails, go back one revision and patch the PCB board or bypass the revision and relayout the PCB.

Check one of the PCB board vendors for gerber file conversion tools.

Hi David, The OP hasn't posted since his first message. I believe from the manner I read his post, he has the Gerber files and a fabrication drawing and that's it. I don't believe he has any PCB files or a PCB CAD tool. Sounds like he got these fabrication files dumped on him with nothing else and now he is trying to get them fab'ed without even an original drill file (or possibly he does have a drill file but doesn't recognize it or it's format).

I always try to pound into designers to do a simple readme text file to be zipped up with their fab files. The readme lists all files, their layer/stackup association, type (Gerber/drill/etc) and the particular data/machine formats of each file. Then nobody ends up in these situations or at least somebody had to do something intentionally stupid for them to end up in this type of situation.

It is possible that one of your gerber files contains images for locating holes, but I would not depend on it.

Bob

Autocad works fine for manual PCB layout. But each program that converts to Gerber from dxf requires its own special format for the drawings. Going from Gerber to dxf for a particular AutoCAD setup requires its own special format out of the conversion program. Going from Autocad to other software also requires its own special conversion software.

Bob