Pulsonix can generate manufacturing data in Gerber, ODB++, IPC-2581. I'd like to use IPC-2581 or ODB++ but I need to know if their implementation in Pulsonix is mature enough compared to Gerber (e.g. current open issues etc) and what format Pulsonix recommend using.
In terms of longevity and widespread use, ODB++ is the one to look at. IPC2581 will also give you a complete manufacturing output but is a more recent addition to the application, and is also less widely adopted by the manufacturers.
We know that many users have relied on ODB++ to manufacturer their Pulsonix boards for years so I would have no hesitation in recommending it, but it will be interesting to hear what some of the forum members think as well.
quote:it will be interesting to hear what some of the forum members think as well.
Currently I output a zip archive containing Gerber X2, Excellon, GenCAD and IPC-D-356 netlist and an ODB++ file. I've been outputting ODB++ alongside Gerber RS-274X since 2004.
The rationale is that the PCB Assember and PCB Fabricator are free to choose whatever format they are more comfortable using. Some fabricators give you a discount on the tooling charge if you give them ODB++.
I've been at the other end, in the mid 1990s, translating the original RS-274 format gerber data with aperture tables of hundreds of apertures and often having to guess the inch/mm, 2.3, 2.4, 3.3, zero suppression etc. into CAM software including Orbotech Image 5000, GC-CAM. It was horrible and the scope for making an error was immense and errors were made occasionally. Extended RS-274X gerber data was a great improvement and greatly reduced the number of errors. I changed jobs a shortly after the fabricator purchased two of the then new Valor Genesis CAM seats that use ODB++ as the native format and importing and editing this format into the CAM system was more time-efficient and easier.
Recently I've been recieving a few quries from fabricators when they've tried to import our Gerber data but I've never had any quries from fabricators that have used the ODB++. The only query I get about ODB++ is "what is it" from a few fabricators and assemblers that haven't come across it yet.
I always check the Gerber in GC-Prevue and the ODB++ in Mentor Graphics ODB++ viewer before it is sent out.
One thing I have noticed recently is a very small number of fabricators that have been passed our data for quote that have claimed to have been unable to read the Gerber X2 format they've been given. I know for certain in one case that the fabricator admitted to me that they were using a very early version GC-CAM that hadn't been updated for more than ten years and I suspect this is the case for the other fabricators since when I've asked them for details about the CAM software they use they've been very silent.
I wouldn't bother about outputting IPC-2581 format at the moment only because there aren't many fabricators and assemblers using it. The idea is a good one - an industry standard that's not controlled by a single company - but it's not prevalent enough at the moment to justify outputting the format. Hopefully that will change in time.
If you're a big company with a high design through-put that uses a couple of fabricators with a very close relationship then it's worth using the format but for medium and small sized companies it's not worth the time at present.