What is the usage of different standards for making gerber file?

[electronc_elementary]

Hi,are there different standards for making gerber file?what is the usage of these standards?
Thanks alot

 

[House_Cat]

barco dpf

ANSI/EIA 274-D is the standard for G codes used for numerical machine control. It is sometimes called RS-274D format. It translates a drawing into a series of ASCII G codes to move a machine for manufacturing. In electronics it is used to control photoplotters for manufacturing masks to be used for exposing photo sensitive copper clad boards to make printed circuits.

RS-274D uses two files for each layer of a PCB. One is the G code file to control movement, and the other is a definition file for aperture sizes. Apertures define shapes which can be drawn by a machine or "flashed" through a pre-defined exposure mask.

RS-274X is the extended Gerber file format introduced by Barco, and combines the apertures into the rest of the Gerber file as well as adding some new G codes to the original standard. You can download a copy of the RS-274X format rules at: **broken link removed**

Modern fabricators generally prefer that you use RS-274X format because of its compatibility with more computer software. The original standard did not specify the exact format for the aperture file, and nearly every design software has their own. It makes loading the Gerbers and apertures more difficult and prone to error. The combined RS-274X format rules standardize the whole file, and eliminates the aperture confusion.

 

[electronc_elementary]

nc files format used in pcb designing

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.

 

[House_Cat]

eia excellon

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.

 

[circuitpeople]

eia standard eia-274-d download

If you're interested in understanding what's in a Gerber file, you might be interestedin https://www.circuitpeople.com. The site will render both the D and X Gerber variants (include aperture file(s) in a zip with the Gerbers if you're using the D variant). Soon it will do Excellon files as well. If you have feedback about the site, I'd be glad to hear it.

 

[House_Cat]

gerbv drill sieb meier

I guess a site like CircuitPeople is OK if you don't mind giving away your board design to total strangers.

It appears to be an anonymous front for some larger company with a half-dozen trade marked names - none of which identifies the true owners and operators, and their motivation. One could surmise that they are trying to develop a Gerber viewer/editor of their own. Perhaps it's a cheap and easy way to gather samples for testing a future product.

If you are dealing with a hobby board, and you don't want to download one of the many free Gerber viewers available on the web, I guess you have nothing to lose. On the other hand, if you install one of the free viewers, you can measure, print, and analyze your Gerber files.