PCB Layout Question

[SteveBull]

Hi.
I am having trouble finding recommendations relating to the minimum spacing betwee the edge of a PCB (PWB) and the tracks or ground/powerplanes.
Any information would be much appreciated.

Steve Bull
Quality and Circuit Engineer.

 

[buzzp]

There really is no rules governing this. It will likely depend on where the PCB will be mounted (dont want something rubbing on your soldermask til it eventually wears through). If real estate is not an issue and there are no other considerations, I use 1/8"-1/4". If you are talking about spacing between two traces or planes then I can get this info if you tell me the voltages. Hope this helps.

 

[uWaveFDL]

I agree with buzzp. Relative to board size, component size and population. I have a VCO board design 0.175 square with max 16 components mounted with 0.012 clearance to outside edge ground plane and a cover soldered to it. The only other recomendation would be keep hot traces away from mounting hardware points. If you are concern is with very high voltage traces with respect to ground plane, there may be a power supply designer in the group that can add more.
I hope this helps some.

 

[SteveBull]

Thanks for the replies, I'm after a general standard that can be applied to a range of products. Our customer (in digital broadcasting) is after setting up a whole load of design rule checks relating to boards, and whilst wanting to get the board as well packed as can be, also wants to guard against damage whilst deblipping, ingress of moisture. I have asked around, and there does not seem to be any specific standard relating to the minimum gap, but the pcb manufacturers I have spoken to suggest 0.3mm (roughly the 1.8" buzzp mentioned) as the absolute minimum.
As I said, any further details(Mil Specs etc.)would be a great help.

Steve Bull
Quality and Circuit Engineer.

 

[SteveSmith]

Get IPC-2221 & IPC-2222 from

http://www.ipc.org,

they are the standards for designing pc boards (pw boards).

From IPC-2222:
10.1.1 Edge Spacing
Except for edge-board contacts, the minimum distance be conductive surfaces and the edge of the finished board, or non-plated through hole, 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 (seeTable 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 requir variances to these requirements. Ground and heat sink planes may be extended to the edge when required by design.

When I design multi-layer boards, I leave at least a .025" gap from power/ground planes to the edge of the board to allow for tolerances so that these do not go all the way to the edge and potentially cause a short.

Regards, Steve Smith
Product Engineer
Staco Energy Products Co.

http://www.stacoenergy.com

 

[SteveBull]

Steve
Thanks very much for the posting, it was exactly what I was hoping for.
Best Regards,
Steve Bull
Quality and Circuit Engineer.

 

[buzzp]

For moisture resistance, get solder mask on your boards when you order and then spray them with 'Conformal Coating' after they are populated. Thanks, Buzzp

 

[uWaveFDL]

If you don't want a heavy coat of Conformal Coat, try
HumiSeal spray. It is a thinner coat but does a very good job as a moisture barrier.

 

[Lewish]

If you are worried about moisture, I suggest you use at least 0.05 inches between plane copper and the edge of the board on inner layer planes. You will always have some delamination of the board material due to the router operation that cuts the PCB out of the panel. Great place to trap moisture.

Lewis