I've drawn a component that has extra vias in it. Basically the device has 5 pads that get electrical connections. But 2 of the pads are very large and the manufacturer recommends adding small holes around the circumference of the 2 very large pads. You can see what I mean on page 10 of the datasheet here: http://www.allegromicro.com/en/Products/Part_Numbers/0756/0756.pdf.
So I used small round vias to make the holes called for in the main large pad. This is in the pcb symbol editing screen. There are 16 of them in each of the 2 large pads.
However, when doing error checking I get 32 no connection errors and 32 pad to pad errors. Is there some way I can exclude these pads from the error checking?
I think that the idea is to increase the number of thru plated pads so that you don't rely on the thru plating of just two big thru plated holes for a high current. Edit your component to have just the 5 pads and then try adding a copper area to "normal" pads for pins 4 & 5 (in the pcb editor) and then add further multiple vias to the copper areas afterwards. Add the vias to the same nets as pins 4 and 5 and as long as the via-via distances is greater than your SPACINGS setting you should be OK.
There is an alternative method if your brave enough to use exceptions !.
In the symbol editor you can add the additional 16 drill holes (pads with same or very slight bigger diameter as drill hole), then add a shape to make the "rounded rectangle with flattened end" as per data sheet on both top & bottom copper layers filled to pad 4/5 !.
Pad's 4/5 can be oval all layers either large enough to overlap the holes or within that area depending upon which solder preference you wish i.e. solder pin to holes or pin & holes !.
Apply pad exceptions to holes not on copper, resist, paste layers !.
Save !.
On PCB editor load the part to which the exceptions should appear in styles !. You must now link all drill holes to same net as pad 4/5 to complete task !. On error check nothing should appear providing pad's are part of a net !.
Advantage is you can move the part without needing special attention to "hacked" vias etc !.
Not sure about newer versions but on V11 you cannot output gerber resist with shapes on the resist layer unless uncheck the pads/resist/paste which defeats the purpose of having over sized resist !!!.
If your version can handle output the resist layer correctly then can add 2 more shapes to symbol on the resist layer if you wish full "pad" as per data sheet !.
Note the radius for R1, R2 & R3 seem to be missing as well as slot width :(.
If you want I could send the library part & a pcb file showing the above from V11 as an example.
Extra pads/vias in a component
Posted - 29 Mar 2013 : 22:48:17
