Flash Symbols ("To Flash or not to Flash, that's the question")

In times of old negative layers for internal power and ground were the norm for most PCB Cad systems. There were some reasons for doing this but the main one was performance as in graphics performance. See with a negative layer the only thing that gets drawn on your computer screen was the actual pads. There was no need to draw a copper pour in the traditional way you would do it. I believe that in Allegro/Orcad the negative planes is a legacy thing similar to other cad tools that have been around for many years.

With a negative layer you had to have flashes in your padstacks for connectivity. 

So today negative layers are not really needed and for internal layers you can use  copper pours just as you would on the outer layers. There are a couple of advantages to using positive layers.

1 You don't have to define flashes in padstacks.
2 On internal layers it is easier to figure out what's connected to a plane and what is not.
3 In Allegro the system can take care of the thermals for you when using positive layers.
4 Making padstacks is a whole lot easier.

I used to use negative layers years ago but not any more. I am not sure why someone would be teaching that as a best practice. I am very much with steve in that the extra work is not needed.

So there is a hidden charm too and something that is not very obvious. When you create your positive artwork and send it off to a boardhouse the boardhouse typically creates "Composites" of your artwork.

A composite is a negative image of your positive artwork. So why they do that ?, well because the photo resist that is used to coat the board is a negative photo resist..

There is a huge advantage in using Negative Photo Resist for boards and it mainly pertains to imaging of the Photo Master. With a Negative photo master areas of the board that are clear "Light can pass thru" will turn out as copper on the board and areas of the photo master that are dark will have no copper.

Needless to say on a board that has a lot of copper the photo plotter will be putting out mainly no dark images so it can plot fast. If using a ink based plotter it means little or no ink is getting put on the photo master film.

I would go with using positive artwork only as a good best practice no matter what PCB tool you use. I would not use Flashes in your padstacks :)

Hope this helps ..

Thanks Scott

There are several other reasons many PCB shops still prefer negative planes over positive ones:  

• As mentioned above, positive planes take more time to process/translate between CAM software and imaging/AOI machines.  This can be managed somewhat through job planning and queuing but becomes a factor when dealing with quick-turns or restarts.
• Positive planes are also more susceptible to data translation errors between the designer and fabricatior (ODB++/Gerber output) and between the CAM software and imaging/inpection equipment which can cause undedected data/imaging defects.  These errors have become less frequent over time as hardware and software have gotten better, however, the increased risk is still there.
• Positive planes, especially split planes or mixed signal/ground planes, take more time to process through the DFM review/panelization process in the CAM department.  Although today's hardware has made DFM checks much faster, the CAM tech usually has more "clean-up" and items to check on a positive layer than a negative layer which adds some time to the CAM/tooling cycle time.
• PCB fabricators will sometimes need to "tweak" (increase) the diameter of an anti-pad independently of the pads to aid in the etching process.  This is much harder to do with a positive plane than a negative plane.  If the design and dynamic shape contraints in Allegro are managed so that enough annular ring and anti-pad to pad spacing is provided to the fabricator then this shouldn't be an issue.

Having been on both sides of this fence (fabrication and deign/layout), I feel positive planes should be used as the electrical integrity of the design is much easier to control and verify within Allegro.  However, its important to manage positive pours so that "clean" data is sent to the fabricatior to minimize the risk of problems.