[Help] Converting Old BoardMaker PCB & Gerber Files to Altium

[yarr]

Hey folks,

I’ve got a bit of a legacy file situation on my hands and could use some input from anyone who’s dealt with ancient EDA formats.

I recently received some PCB design files that were apparently made in BoardMaker (possibly version 2 or 3—not to be confused with the educational software). Unfortunately, I don’t have access to the BoardMaker software itself—just the exported files.


What I have:

A .pcb file (assumed to be the PCB layout)

Several “001” and "N01" and "SIZ" -type files, that look like Gerber files, but with nonstandard extensions


I can't open the .pcb and gerber-like files are giving me trouble.

My end goal is to get PCB layout design into Altium Designer (or possibly Protel), hopefully without manual rebuilding .


Questions:

Has anyone worked with this specific BoardMaker format before?

Are the .001/etc files likely to be RS-274X Gerbers, and can they just be renamed to .gbr and viewed in modern tools?

Any tricks to opening or converting .pcb files from BoardMaker into something readable (Protel, Altium, etc.)?

Is there any known freeware or toolchain that can assist here without needing the original BoardMaker software?
Bear in mind, I am dealing with some company property pcb's.

And worst case—any recommendations for third-party services that can handle this kind of conversion?
I’d rather avoid sending it off unless it’s absolutely necessary, so I’m trying all options first.


If it helps, I can post some file samples or screenshots of what’s inside the .001 file (it’s ASCII and seems to have %FSLAX codes and aperture definitions).

Thanks in advance for any insight!

[Kean]

You are likely out of luck doing anything with the raw pcb file.  If the other files are ASCII and contain %FSLAX and similar then they are almost certainly based on some revision of the Gerber format.

Any idea of the year the files were created?
What trouble do you have when trying to view the gerber-like file?

You could try viewing them in the "official" Reference Gerber Viewer at https://gerber-viewer.ucamco.com/

No idea how well that will work with old or non standard files.  There have been many changes over time to the Gerber format, which might cause a current viewer to have trouble with a really old file.  You can check out the latest format spec and some details of the evolution/deprecation of the format at https://www.ucamco.com/en/gerber/downloads

Unless someone comes up with an old but working version of BoardMaker, you are almost certainly better off just recreating the PCB layouts from the Gerbers using Altium or KiCad.  There are some other threads here and on Google about best way to do that depending on what release of Altium/KiCad you are using.  It would help you significantly if you have a sample PCB or some original paper prints of the layout to verify the files against.

[yarr]

Hi Keane,

Thanks again for the helpful responses so far. I have checked it out.
It’s a shame about the .pcb file being likely unusable. But if I understand you correctly, it might still be possible to reconstruct the PCB board from the old Gerbers?

Responding to your questions:
-All the files are from 04/2008.
-After digging further into the files, I’ve confirmed that the PCB files I’m working with are in RS-274D format, not RS-274X (as I have mistakenly stated initially). I opened some of the .001 files in a text editor and found they contain plain X/Y/D commands like this: "X2065Y1142D02*" . There are no %FSLAX or similar RS-274X extended format commands, confirming it's an older Gerber format that needs an external aperture definition file.

Good news is that I found a manufacturing build sequence sheet, and it includes:
 
Layer assignments (e.g., XXX-1.001 = upper track, XXX-8.001 = lower track, etc.)
An aperture table file named XXX-A.001
Drill files (EIA: .DD.001, ASCII: .NC.001)
Drill tool report: .NC.SIZ

So I have what I believe are all the necessary files, but I’m not yet sure how to use them properly to either view or import the board layout into Altium Designer.

When I rename all the "potential gerber files" to .gbr. and and changed default import gerber setting to RS-274 Altium, it just doesn't do it fully correctly. It's hard to explain and every layer is showing slightly different things (surpirse surprise). One interesting thing is that the upper and bottom silk screens look normal and Buried track looks peculiar to say the least (see attachment).

I might be doing something wrong though systematically, so please tell me how you would approach this situation with all that information.

[Kean]

Yes, I was suspecting some of the files might be RS274D (aka Gerber X0) which was replaced by RS274X (aka Gerber X1) in 1998.  I've been fortunate never to have dealt with those files.

A little bit of research brought up an older website that may help

1) This document which explains the change from RS274D to RS274X, and could be useful for manual modifications to combine the apertures and other new definitions with the layer files
https://www.artwork.com/gerber/274x/rs274x.htm

2) This software which seems to support merging the aperture data and layer and saving to an RS274X file.
https://www.artwork.com/gerber/gbrvu/gb_index.htm
It is old software originally from the 90's but still seems to be maintained and supported.  I think may be free to try, but is not free to use.  There is a Download link on that page and pricing link in the page footer.

Step by step instructions... https://www.artwork.com/gerber/gbrvu/faq/274d274x.htm

Have a dig around that site and you might find some additional info, but I suspect for a one-off you might be better reading the first document and doing the file combining manually.

No idea on the drill files, but I suspect they will be comparatively easy.

I suggest starting with the board outline first, then only view the outline plus one other layer at a time.  Maybe with the drill data as well.

Once you have usable Gerber data, you can try various methods to generate an editable PCB in Altium.  I've never tried it, but I suspect it will depend on your Altium version.

Do a google search on "altium gerber to pcb" and you'll find a bunch of links that may help.
https://www.altium.com/documentation/knowledge-base/altium-designer/convert-gerber-odb-fabrication-data-back-to-pcb

[Doctorandus_P]

Once upon a time I was playing with some old Gerber files, and it did not make much sense in a Gerber viewer. Then I hacked in a line of code to toggle from absolute to relative coordinates (or it was the other way around), and suddenly the Gerber did look like something plausible.

For the rest, I only use KiCad. KiCad can (re-) create a PCB from a set of Gerber files, but the conversion is only partial, as a lot of the needed info is simply missing from the Gerber files (for example, there can be pads in a Gerber file, but there are no footprints). A KiCad project can apparently be converted to altium, but apparently this does not work very well