Negative Gerber Conversion-Need Information

converting negative plane to positive plane

Hi,
I recently got a gerber file from our client. I am converting back to PCB form in protel. The Gerber file is in negative form for the power planes. I want to convert the Gerber to positive form so that I can do editing on that. Can anybody help me how to convert the Gerber to negative.
Thand and Regards,
Vamanan Kutty

negative

You could try and import it into a copy of GCCAM etc and then export it back out as positive.

Look for a Gerber editing software.

pcb gerber plane negative image

I think CAM 350 is better for these type of applications

The negative format for the plane is the normal way a plane is represented in EDA software. In Protel, the planes are displayed in negative, and you edit them by placing lines and fills where you want copper removed. It is done this way in all PCB software to reduce the size of PCB and Gerber files.

There is no need to convert the normal negative planes to positive planes. Positive planes are not the way it us usually done. If you reverse engineer the board to create a PCB file, the planes will convert to the normal format used by Protel - that is negative planes.

It appears that you believe you must used polygon pours to make a plane - this is not true. Polygon pours are used to create unusually shapped copper areas, but not for covering an entire layer to create a plane layer.

House_Cat,
I want to say that the Gerbers are in positive format. I want to convert into negative so that I can edit in Protel.

vamanan said:

House_Cat,
I want to say that the Gerbers are in positive format. I want to convert into negative so that I can edit in P*otel.

Click to expand...

I'm afraid you're going to have to do the work manually. If all you have is the Gerber file, there's not enough information to change a positive plane (polygon copper flood) to a negative plane. A Gerber file represents a positive plane as hundreds or thousands of small parallel line segments - there isn't anything in a Gerber file that identifies consolidated regions of copper.

If you have a netlist or ODB++ file for the board, you could do a reverse engineering PCB import using CAMTASTIC - the positive plane would be imported as copper flooded areas on a signal layer. In the PCB editor you would use the positive copper flooding as a template, then change the display to show only your new negative plane and the imported layer. You could then trace your new negative plane split lines over the image of the imported layer. You would have to assign the appropriate nets to restore the connectivity.

With only the Gerber files and no net information, all you can get is imported primitive line segments in the PCB editor. Every connection would have to be manually defined.