Throughhole near pcb edge, how close is too close.

[Psi]

Hey, i want to mount one pcb onto another at 90degrees using a typical 2.54 pitch right angle header.

The issue is that the holes need to be quite close to the edge on one of the boards and i'm not sure if they are too close to get manufactured.

Is there a rule of thumb or formula for how close a hole can be to the edge given its size?
I'm going to be using PCBcart and i've checked their website but it doesn't mention it.

I'll probably end up emailing them but i thought id ask here as well.
The holes on my board will be 0.7 or 0.8mm and need to be 0.8mm from the board edge for the header to fit flush on the board.

[codeboy2k]

This is the specific kind of question you should ask the manufacturer.

However, it usually doesn't matter, often small SMD carrier boards are manufactured with plated through holes that are then cut in half, to make a solderable carrier board, with
holes on the edges that are half-plated in a semi-circle now.

Your board is likely going to be panelized, so there is plenty of extra board space at the edges of the panel , and they can drill and plate anywhere on your board. 
It will be cut out later.

--Cheers!

[metalphreak]

The accuracy of the final routing should be similar to the registration tolerance for drill holes (if they don't mention routing tolerance separately).

For example, Seeed has "Registration (Mechanical): 0.09mm ". Combine this with the minimum line/pad spacing to work out how close to the edge you can safely go. Some places also spec a minimum ground plane pullback from the edges (ie 10mil) so you could also take this into consideration.

For a header connection on the edge, if a little bit of the pad is routed off it shouldn't matter too much. You just have to worry about the mechanical strength of the PCB.

[Short Circuit]

However, it usually doesn't matter, often small SMD carrier boards are manufactured with plated through holes that are then cut in half, to make a solderable carrier board, with
holes on the edges that are half-plated in a semi-circle now.

For a header connection on the edge, if a little bit of the pad is routed off it shouldn't matter too much. You just have to worry about the mechanical strength of the PCB.

Actually, this does matter quite a lot. Almost no manufacturer will make boards which have the risk of holes being cut open by the routing process.
Of course, it can be done, but it requires much more attention by the manufacturer to prevent the plating to be damaged or even ripped out of the hole.
And as usuall, more attention means more cost, and usually not available on simple pooling services.

As for this specific situation, use the smallest hole possible, so that would be the 0.7mm. This is finished hole size, so the actual drill will be 0.8 or so. this means the hole is 0.4mm away from the edge. If the edge is routed (instead of scored / V-cut), then this shouldn't be too much of a problem.

The folks at Pcbcart are very communicative, so just order the board and send the files. And wait for any comments, if any. Also, often it helps to ask if the issue(s) they raise are really, really a problem; Sometimes they agree the issue "shouldn't" be a significant issue for production, and simply proceed. Or maybe they'll charge a bit extra for tighter manufacturing tolerances, in this case probably because of a reduced annular ring.

[Psi]

thanks everyone

That answers my question nicely

[metalphreak]

If you want open end half pads (whatever they're called) like: http://www.seeedstudio.com/depot/images/large/product/newblue_LRG.jpg

Someone asked in the forums if they could do it, and they said yes, but for an additional fee. You just have to send them the files and request a quote.

[Psi]

na i just wanted to put them close to the edge.