Protel Gerber File format

[changzhi]

Hi, In DXP 2004, I used 'Fabricate Output'->'Gerber Files' to generate gerber file. The output can be loaded by DXP2004 and Protel99, but the PCB foundry got errors when loading them. Looks like protel used some custom apertures that the foundry's software cannot read. Do you know anyway in Protel to disable the function of exporting designs as blocks? Thank you very much!

 

[House_Cat]

You probably used solid polygons in your design, and your fab doesn't know how to use the Gerber codes for them. They must have old software and old equipment.

Go back to your board, and change all the solid polygons to hatched polygons. Then output a new set of Gerber files. That should satisfy your fab.

Protel doesn't use any custom features in their Gerber files. All of the apertures and G codes are from the RS-274 and RS-274X standards. I've been using Protel software since they started the company, and never had a problem with the Gerber files.

 

[Johnson]

I had same problem, it solved by "change all the solid polygons to hatched polygons"!

What is G codes?

 

[House_Cat]

Re: P*otel Gerber File format

What is G codes?

If you open a Gerber file in a text editor, you will see lines that begin with the letter "G" followed by a number. Those lines are instructions to the Gerber plotter on what to do. The X, Y lines that follow the "G" line are the coordinates to be used for the action specified by the G code.

In the case of filled areas like polygons and planes, there are two codes, G36 and G37, that allow more efficient definition of the filled area. These are the two G codes that your fab apparently can't use. Modern photoplotters and software use these two codes to define "solid polygon regions". Older software and equipment may not be able to properly interpret and display these regions, and have to rely on an array of thousands of line segments to define the filled region.

 

[Johnson]

P*otel Gerber File format

does the pcb designers needs to know and understand the g-codes?
in gerber files how origin is declared by g-codes? how the type of reference: absolutely or relative , are defined?

 

[House_Cat]

No - a PCB designer doesn't have to know the Gerber G codes. It's just one of those things that a person learns over a career of designing printed circuits.

The Gerber users manual describes how information such as the origin is defined in the file. You can download a copy from:

**broken link removed**

or

**broken link removed**