What is the default Internal Plane polarity? Negative or Positive??

[zust4you]

Hi Guys

I ordered a PCB with 6 layers which had two internal power planes. Both the internal power planes were negative and the remaining 4 signal layers were positive. When I ordered the PCB there wasn't any option for me to select the polarity of the layers, and now I have PCBs with both the internal power planes not working. They basically treated everything as positive and made the PCB.

My question is what is the default polarity of the internal power planes? Was I responsible for letting the manufacture know that the internal power planes were negative?

Your help is greatly appreciated.

Thanks

 

[HMS1021]

I have only used two suppliers for about 30 new designs. With both suppliers I only supply positive Gerbers and they adjust depending on the layer side they are fabing. Based on your experience I'll be sure to find out what a board shop expects should I try a new vendor. They do not appear to look at the art, I once up-loaded the top overlay for a Layer 2 GND plane, they fabed it and I paid for my mistake. Since then I now send a fab drawing with callouts and even pay for a design check on the more complex boards so I have a bit stronger claim if they fab a useless board.

 

[Mattylad]

Zust, it is your responsibility to ensure that the data you provide is clear an unambiguous.

Also to choose a manufacturer of your boards that does proper checks etc.

 

[FvM]

To refer to the initial question, there's no general default power plane polarity, different CAD tools have their preferences.

Negative plane artwork has some details that normally reveals it's nature, e.g. an outline has to be included to isolate the plane from the board edge. There are also commonly used file name syntaxes that designate the different gerber layers. For this reasons, I don't remember a similar misunderstanding as described in your post, even with hasty and sometimes poorly specified prototype jobs.

But it's clearly suggested to add a describing file to the gerber data that includes a full stackup specification, layer description with gerber file names, substrate thickness, copper weights, surface finish, special process details.

 

[marce]

Use positive artworks for your final data, and never ever mix polarities'.
negatives were used initially as PC's did not have the power to handle positive planes. Now they do and most designers will use templates on the power plane layers to indicate the areas for the copper pours. During the design cycle set the planes to negative (it speeds up the design flow), then when all signal routing and power stubs have been done, change the power layers to positive, copper pour and do a DRC check.

- - - Updated - - -

Further, if you are sending out Gerber and excellon data, always send out an IPC-D_356 netlist for the manufacturer to check your Gerber's to, this will avoid these mistakes.