IPC-A-600 is a visual guide to help evaluate bare board acceptability per IPC-6012.
Its only concerns are for the rejection criteria that are RELATED to the edge-to-conductive feature distance; like nicks, haloing and crazing.
(see IPC-6012 3.3.1)

I think what you are looking for is in the IPC-2222 Design Standard 

10.1.1 Edge Spacing Except for edge-printed board contacts, the minimum distance between conductive surfaces and the edge of the finished printed board, or a NPTH, shall not be less than the minimum spacing specified in Table 6-1 of IPC-2221 plus 0.4 mm. Printed boards that slide into guides shall have a minimum external conductor to guide distance of 1.25 mm or minimum electrical clearance (see Table 6-1 of IPC-2221), whichever is greater. Special design applications in areas such as high voltage, surface mount, and radio frequency (RF) technology may require variances to these requirements.
Ground and heat sink planes may extend to the edge when required by design.
Design should provide sufficient edge spacing to avoid unnecessary haloing and crazing rejections. Rejections can occur when the edge defect is greater than 50% of the clearance to edge spacing. Brittle material or heavier glass weights increase this risk.

What bothers me a little bit about the text above is that the first sentence contain a SHALL (or more specifically, a SHALL NOT), 
and then a following sentence says "Ground and heat sink planes MAY extend to the board edge when required". 

The proposed text for the next IPC-6012 acceptability document says:
When edge spacing is not designed in accordance with IPC-2222, evaluations for nicks, crazing and haloing shall be AABUS. 

I'm predicting some extra AABUS discussions (between User and Supplier) when designers start sending data that has copper planes extending all the way to the board edge, because some well-meaning engineer or supervisor claims it is "required". And when the designer gets questioned why he would do such a thing (board routing tolerance will certainly leave exposed copper on one board edge or the other, and possibly smear the planes together, unless the fabricator modifies the data to get a reasonable minimum clearance) he will simply state that the design IS in accordance to IPC-2222, because it says the designer MAY do this if someone claims it is required. But that's probably not the question you were asking...

sorry for the delay in responding,
onward thru the fog!
Jack 


On Thu, 17 Dec 2015 19:22:56 +0000, Victor Hernandez <[log in to unmask]> wrote:

>Fellow TechNetters:
>
>   I cannot recall chapter and verse on above IPC criteria that a copper conduct can come close to the laminate edge,  Especially Pwr.
>
>Victor,