gerber6x00 negative plane island

Hello,

For negative split planes to output correctly using Gerber6x00 you will need to ensure that all the planes find a way to the board edge via the splits, in other words you cannot have a smaller plane inside of or totally surrounded by another plane.  Basically, it treats the opening in the larger plane as a void during artwork generation.  This is only an issue with Gerber6x00 and not an issue with Gerber 274X (as you probably already know)

I have a couple solutions:

1) Break the larger plane so that it doesn't totally surround the two other planes such that the two planes have a path to the board edge. See attached image for two possible break points (Red break line option 1 and Purple break Line option 2 - you don't need to do both)

2) Enable "Suppress Shape Fill" in your Artwork Control Form for this particular layer, here are the steps to do this successfully:
        A. Separate all of the split planes on this layer and trace the board outline using Lines drawn
            on Class Anti-Etch/Subclass <split plane layer name>.
           These splits will be used to separate the different nets.
        B. Update the Film Record for this layer so it includes the Lines drawn
             on Class Anti-Etch/Subclass <split plane layer name>
        C. Enable "Suppress Shape Fill" for this particular layer via the Film Record.

Solution 1 is the preferred solution but your customer may not like doing this.  You can always offer to add stitch vias on each side of the split lines and add a shape on another layer connecting them together in an attempt to bridge the gap over the split.  It is always best to have continuous planes but depending on the plane connections it may not have that much of an effect to add a couple splits.

Solution 2 is something that can be done to address the issue but is very dangerous because the Lines drawn on Class Anti-Etch/Subclass <split plane layer name> have to be done exactly correct and if you update your split plane shapes you will need to manually update the Anti Etch Lines to match.  You will not get any notification if this split lines are done incorrectly and you could possible short a pin/via to the wrong plane. (NOT PREFERRED but you may not have a choice if the customer does not like Solution 1.

The perfect solution would be to generate RS274X Gerber which handles this correctly and the issue disappears but it sounds like your customer wants to output Gerber 6X00

Hope this helps,
Mike Catrambone
Plexus Engineering Solutions 

 Hi Mike!

While waiting for reply yesterday, i was doing some experiments on how to output the proper gerber for gerber6x00.

For the first solution you offerred, i recommended it to the customer but the customer did want to break the plane. And the customer insisted on gerber6x00... (because they used old manufacturing plant). Here in Japan also, most customer use Allegro 15.2 and 15.7 version. Only few customers use version 16 and up...And this is my first time outputing gerber using 6x00 (fuji electric designs).

What i did was the 2nd option. I added a cutline in the antietch same size as the clearance (shape to shape clearance). At first I did not know the function of Suppress shape fill, but while exploring all options, I check it then successfully generated a gerber data for the Power layer. Im not really sure if it was the correct method. 

Thanks to your explanation, I guess i hit it right. Though I did not know the consequences ("dangerous"), when doing cutline method.

You are really an  expert in Allegro.　Thank you for the detailed explanation. I learned a lot from this design though it took me 1 day to generate the gerber data. ^_^

Arigatou Gozaimasu!

eric

NEC Toppan Circuit Solutions, Inc.