Combining Gerber positive and negative files into a single G

[Paul]

My pcb layout program generates traces as a positive Gerber file and
the ground plane as a separate negative Gerber file. Is there a
simple way to combine the two so that there is only one Gerber file
for each layer?

Thanks,

Paul

 

[Brad Velander]

Paul,
First, what program are you using? Someone may know how to do
it if they knew which program you used. If it has to be done via
merging Gerber layer, it is not extremely difficult but it is not
simple. I have never done it myself but I realize the steps
required to do it at a Gerber level.
Possibly your fabricator could do it more easily than you.
Their tools are sometimes more sophisticated for these
operations.
I am really curious about which tool you use because I can't
see this being a useful tool unless there is just something in
the set-up that you missed to do it in one file.

--
Sincerely,
Brad Velander

"Paul" <linsay@linsay.com> wrote in message
news:ccb0f593.0405031342.7c3612e6@posting.google.com...

My pcb layout program generates traces as a positive Gerber
file and
the ground plane as a separate negative Gerber file. Is there
a
simple way to combine the two so that there is only one Gerber
file
for each layer?

Thanks,

Paul

 

[qrk]

On 3 May 2004 14:42:46 -0700, linsay@linsay.com (Paul) wrote:

My pcb layout program generates traces as a positive Gerber file and
the ground plane as a separate negative Gerber file. Is there a
simple way to combine the two so that there is only one Gerber file
for each layer?

You don't say what program your using.

I don't understand your question. What you describe is normal. Layers
defined as planes are normally plotted as a negative, trace layers are
plotted as positive. These are separate files because they are
separate layers.

Are you talking about a single layer having traces and plane area(s)?
In this case, you would create your plane areas using pours. If you
ran a trace thru the pour, your layout program should carve out a
specified clearance around the trace. The resultant Gerber file will
be a positive with lots of black for the plane pours.

Perhaps you are not familiar with your program or the program has
limitations. If your program has limitations and you need to combine a
trace layer with a negative of a plane layer, have the pcb house do
this. PCB houses have full blown Gerber editors which allow them to do
fancy things like this.

Mark

 

[Geo]

On 3 May 2004 14:42:46 -0700, linsay@linsay.com (Paul) wrote:

My pcb layout program generates traces as a positive Gerber file and
the ground plane as a separate negative Gerber file. Is there a
simple way to combine the two so that there is only one Gerber file
for each layer?

Sounds like Cadstar (DOS).
In which case the answer is no. Tracks on a plane are plotted at normal size on
the positive and (width + 2*clearances) on the negative.
You simply tell the pcb manufacturer to combine them.

Geo

 

[Paul]

Thanks for the comments. I use a layout program and Gerber file
generator made by Douglas Electronics. My problem came about because
I'm trying to use a budget online pcb fabricator, pcbfabexpress.com,
that requires that the files be combined and doesn't do it for you.
After writing this comment I was able to figure out how to combine the
Gerber ASCII files after spending some time reading the Gerber RS-274X
documentation. I combined, in order--very important--, the negative
plane layer followed by the positive trace layer. I cut the redundant
header information from the positive trace layer and added the
instruction %LPD*% just before the positive drawing instructions.
This instruction tells the plotter to draw dark traces unlike the
previous negative layer where it was instructed to draw clear traces.
This worked fine and displayed properly in ViewMate. If you reverse
the order and do positive followed by negative using %LPC*% (= draw
clear), the positive traces are overwritten by the negative ones.

linsay@linsay.com (Paul) wrote in message news:<ccb0f593.0405031342.7c3612e6@posting.google.com>...

My pcb layout program generates traces as a positive Gerber file and
the ground plane as a separate negative Gerber file. Is there a
simple way to combine the two so that there is only one Gerber file
for each layer?

Thanks,

Paul