eia excellon
electronc_elementary said:
Hi HOUSE_CAT
your explanation was very useful but how about (Barco DPF OR Fire 9XXX OR HPGL OR EXCELLON OR SIEB& MAYER ).
Thanks alot.
Those are not Gerber formats. They are complete board files, NC drill, or plot formats.
HPGL is "Hewlet Packard Graphics Language" for plots. It is strictly a plotting language, and is not a Gerber format.
Barco DPF is "Data Process Format" and is an early attempt at a standard way of sending PCB information, including the netlist, layer plots, etc. IPC tried to replace it with GENCAM, but couldn't get the industry to accept it. Valor's OBD++ is the current favorite as a replacement. Again, it is not a Gerber format - it is a complete board file containing all the data about your board. It's just like the file you get from your EDA software, only in what Valor and IPC hopes will be a "standard" format. Some fabs can generate Gerbers from a Barco DPF file, and most can generate Gerbers from ODB++.
Fire9xxx is a model series for CSI brand laser photoplotters. Data in that format is intended only for those photoplotters, and would have to be translated to standard Gerber format for most fabs to use - unless they happen to have a CSI plotter.
Excellon is a drill file format similar to Gerber, but used only for controlling CNC drill/mill machines. It is an ASCII format like Gerber, but uses different codes and data format for controlling drilling and milling machines. You can see the program commands at : **broken link removed**. It is the most common NC drill and mill language used by PCB fabs.
Sieb and Meyer is another drilling and milling machine programming language developed by Sieb&Meyer for their CNC machines. It is seldom used for PCB fab submissions because it is a binary file, and has to be translated to the specific Sieb and Meyer machine in use. Even companies who use S&M machines prefer to get the Excellon ASCII file and have their software convert it.
There are only two real Gerber formats RS-274D and RS-274X. Gerber is capitalized because it is a proper name - it is a very specific data format used for making a photoplot. In addition to the Gerber files, you need NC Drill files to make a PCB. Those files are in Excellon, EIA 244, or Sieb and Meyer format. Excellon is the preferred format.