ODB++ output from Eagle Pro?

Hello,

Do you know how i can get an ODB++ output from Eagle PRo?.....the pcb house have asked for this...i have already sent them gerbers and drill file..but they now want ODB++.

Eagle doesn't do ODB++ and the last time I looked (a month or so ago) there were no plans to.

Keith

Thanks Keith............is there a way of using the gerbers to get an ODB++ file using some external program.?

Also, does Eagle do anything similar to ODB++?

I guess it should be possible to produce ODB++ from Gerbers but I suspect it will only be with some costly software. I have never found it to be necessary because I have never come across a PCB house which cannot make a PCB from Gerbers!

Keith

Extended gerber is still the industry standard, I think. I understand that PCB manufacturers might prefer ODB+, but I presume, that they are required to accept gerber in the foreseeable future.

Its the PCB assemblers who want the ODB files.
Its for seeing the coordinates of the components.

Eagle can give me a component coordinate file, but the pcb assembly house says that this isn't useful since we might not have put the component origin in the middle of the component, and also, the "rotated" notation is confusing to them, as where is it "rotated" from?

So our pcb assemblers are very good, and very professional, they are called asteelflash, and they want ODB files, -how can I get ODB files from Eagle Pro?

They say they can do it without the ODB but its more time consuming and expensive.

this isn't useful since we might not have put the component origin in the middle of the component, and also, the "rotated" notation is confusing to them, as where is it "rotated" from?

Click to expand...

In other words, it's a problem of assembly file quality. Rotation of components (e.g. rotated from orientation in tape reel) also occurs in ODB++ files and has to be recognized. The information content of ODB++ also depends on the component library quality, in so far there's no big difference to classical assembly files.

Apparently Eagle doesn't support ODB++. There are commercial gerber tools that can generate it, but they cost some money and have to be learned. As long as you don't schedule a new PCB design every week or so, it won't pay.

depends on the component library quality

Click to expand...

the thing is, what one person thinks is a quality library part, another person will say that's the wrong way to do it...etc etc.
So I wonder what way you have to do it to be able to give a useful ODB file?

I always put the component origin in the geometric centre, -that's fine for 0603 resistors, but what is the component centre for say a DPAK fet?....I suppose some would draw a rectangular "courtyard" round the footprint and then say its the centre of that rectangle, but goodness knows how a pick and place machine picks up a dpak fet and somehow is able to find that point.

Another point about eagle is that when I export a "partslist" from the layout editor, it puts brackets round each coordinate..........and I then have to go through the text file and delete every single bracket, which takes ages given there are 100+ components......also the Cartesian coordinates have a space between them (between x and y values), but the space doesn't line up down the text file, so I have to cutnpaste each y coordinate into a separate column.....this again takes ages.

Asteelflash are emphatic about needng ODB, (so are other EMS's) and I would be willing to pay ten euros or so for a bit of software to derive the ODB file from the gerbers. I imagine the ODB is just a sort of graphics file

ODB++ is the best way to get PCB data manufacturer, IPC-2581 will be better if it ever gets global acceptance (Currently I believe Lockheed are the only major user.) and Gerber suffices though it is a pain to create a manufacturing pack.
For PCB libraries you should be following IPC-7351, SMD PBC component creation as had a set of rules that have worked since I started with SMD in 1988.

ODB++ has the artwork data, similar to Gerber data (vector artwork information), drill information and it also has inbuilt intelligence with both footprint data and electrical connectivity, so the manufacturers can confirm the artworks are correct during DFM without the hassle of reading in an IPC-D-356 netlist.
When you do a HDI design with 6+ layer pairs for the microvias, then you really appreciate the ease of ODB++

It seems to me that your choices are:

1. Tell the manufacturer that you cannot produce ODB++ files and to get on with it.

2. Buy a software package that supports ODB++ and recreate your schematics and PCB layout(s).

3. Find another manufacturer (there are lots of them).

Also, removing parenthesis shouldn't be a big deal (with text find & replace), even ignoring the fact that the Eagle ULP is flexible enough to create things in any format, I would have thought.

Keith

Search and replace is easy even on large files, search for "(" and replace it with "" - do not include the parenthesis.

This Treez, is one of the reasons why some go for the higher end packages, because it does the higher end stuff that people want.

It seems to me that you may need to learn more about how to output the pick & place file, also make sure that your component origins are central.

If Eagle wont do it - look at getting GC-Place to take your Gerbers and produce an accurate placement file based on the component pad layouts. (Hint - that will cost more than other packages.)

By the way, if the manufacturers have decent equipment then the centroid location is often just a rough suggestion to them, they use optical systems to align on the pads if needed and then they can correct the program.

If they complain that they have not got ODB++ from you then tell them to shutup and get on with it or you'll take the job elsewhere.