274D vs 274X

[Dan]

Could someone please tell me the difference between the two, and why I should use one over the other???

thanks,

Dan

[Tom]

Dan,

Gerber 274D has been around for over 30 years, while the 274X has only been around for the past 10 years. The only difference between the two formats is that in the 274D (old format) requires the aperture lists (.REP files) to be provided in a separate file. You'll have the Gerber file and an aperture file. The newer 274X format has the apertures embedded in the Header of the Gerber file, so you do not need to provide a separate aperture file (.REP file).

The only confusion in this is that PowerPCB produces aperture tables (.REP files) for both formats. When you produce 274X it is not necessary to provide the aperture tables. As a matter of fact it causes confusion when you do. When you process Gerber files using 274X, we always delete the aperture tables (.REP files).

PowerPCB should have an On/Off button for producing aperture tables when using the 274X format. It's always a hassle to remember to delete the .rep files.

[Dan]

Thanks Tom,

Which format would the fabrication shops care to have? Would it make any differnce to them???? Does the fabrications CAM department still put this information in by hand or is it automated some how, but having it already built into the Gerber file?

Sorry for so many questions all in one shot.....

Dan

[Mark Larson]

The seperate aperture file is no longer the issue it once was, reading the aperture file is automatic. Of course having a seperate file means the possibility of sending them the wrong one or not sending it. You also have to archive the extra file. But using X leaves you open to many more possibiliteies of bad Gerbers, X files are more complex so they have greater possibility of being written or read incorrectly. To each his own, I use D.

[Tom]

Dan,

We used 274X exclusively (since PADS fixed a 274X bug back in PowerPCB 2.0 when they first released it).

Mark's correct that manufacturers don't care which format you use. It does not make any difference to them.

As a matter of fact, we don't use Gerber data anymore. Haven't used it for over a year. We have CAM350 and only provide ODB++ data. If you ask any manufacturer what they prefer they will all tell you ODB++ is better than Gerber (if they have Valor front end software).

[Dan]

Thanks Mark and Tom,

Tom,

Could you elaborate on ODB++? I've never heard of it.

Dan

[Tom]

Dan,

ODB++ was invented by Valor. Most PCB manufacturers use Valor software as their CAM tool. You can get a free ODB++ viewer on their website http://www.valor.com/ . Just click on the VUV ICON.

Gerber data will be completely replaced by ODB++ in the next couple of years. Gerber will become obsolete.

ODB++ is one single file that contains all the intelligence of your native CAD database. Cadence and Mentor have been creating ODB++ for some time now. I'm totally shocked that PowerPCB cannot output ODB++ data. Flextronics Corp. just created a program that translates a PowerPCB ASCII file into ODB++, but Innoveda can't do it????

The ODB++ file contains:
Copper data for direct imaging (on photoplots required)
Solder mask data that can be instantly adjusted
The CAD database netlist
The NC Route data
The NC Drill data
The Drill Drawing

ODB++ data shaves hours off the front end manufacturing CAM process because the imported data has all the layers completely lined up with the drill data and completely named and colorized. All the CAM operator has to do is push the DRC check button and it runs a complete DFM analysis and produces an error report (if their are any errors).

There is no need to provide an IPC-356 netlist, apertures, Gerber files, drill data or a readme file. Everything is completely aligned in one single file. This is a major technology advancement and it will dramatically improve productivity levels, reduce errors and hopefully reduce cost.

I can't wait until PowerPCB has ODB++ output. You would simply select File/CAM/ODB++ and you're done.

[Dan]

Tom,

This ODB++ sounds like GENCAM..... what ever happed to GENCAM? I thought that was going to be the way of the future? I guess not?????


Dan

[phillipr]

Tom

Are you still using cam350 to convert your files?
Did the split/mixed plane issue ever get resolved?

[Mark Larson]

Here is a comparison I'd like to see: A sample GenCAM file and a sample ODB++ file of the same data. I have seen GanCAM files and they made my head swim. If I made a simple board, an SOIC-8, perhaps a chip capacitor and a SOT-23 with some traces put down and perhaps a piece of text could somebody then create the files?

I think if people saw sample files it would go a long way in seeing the advantage of the new formats. The importance of keeping the file simple cannot be overstated.

[Tom]

Dan,

You're not following the thread on "GenCAM & ODB++". They're converging together into one format and will be called something brand new. In two years, both GenCAM & ODB++ names will be gone and the new (un-named) format will take over.

Here's the link to the convergence thread.....

http://www.pcbstandards.com/forums/showthread.php?s=&threadid=595

[Tom]

Phillip,

Are you still using cam350 to convert your files?
The only issue that we are having trouble with in CAM350 is that when you convert Copper Pour areas from Draw to Flash there is a bug. We are working with DownStream Technologies with this issue.

Everything else converts perfect. Currently, we only provide ODB++ data to all our manufacturers. We use Split/Mixed planes on some designs, but we mostly use "Custom Thermal" planes.