Solder Mask Sliver Constraint problem - Page 1
Forum section: electronics / general

author: ElektroQuark
author_rank: Unknown
timestamp: August 28, 2014, 09:11:38 am
content: Hi:Why is there a problem here (see image)?Shouldn't the solder mask be extended so it is continuous without gaps in the final PCB layout?How can I solve this? Slivers are too tiny to low constrins limit further.

author: AlfBaz
author_rank: Super Contributor
timestamp: August 28, 2014, 10:30:43 am
content: QuoteIt is. What this is flagging is the limit on how thin the "sliver" or strip of solder mask is between padsYou need to check with your PCB manufacturer to see how small a "solder mask sliver" they allow. You can then set you "Minimum Solder Mask Sliver" appropriately in your design rules. If the "sliver" is to small, chances are it will simply peel or flake off when soldering or even handling. The other option is to reduce your solder mask expansion (the purple area around the red pad) but again, depending on your pcb manufacturers tolerances, you run the risk of having some of the solder mask on the solder pad itself

author: rs20
author_rank: Super Contributor
timestamp: August 28, 2014, 11:47:30 am
content: Quote from: AlfBaz on August 28, 2014, 10:30:43 amAs a general rule (and especially, judging from the picture), I feel reducing the solder mask expansion (equal to or close to manufacturer tolerance) is thefirstthing he should do -- you don't want your solder mask expanded any further away from the copper than you can safely get away with, even in a design where ERC already passes. And of course, you should be setting the minimum solder mask sliver according to manufacturer tolerance as well; but this is less important in some sense because solder mask expansion has a direct impact on the gerber files and the PCB you end up with, whereas minimum solder mask sliver is just a ERC check thing.If you still have the error after setting both rules, then your manufacturer can't handle a component with a pitch this fine (without resorting to funny hacks like a) just ignoring manfacturer limits or b) making your pads thinner, both nasty things to do).

author: AlfBaz
author_rank: Super Contributor
timestamp: August 28, 2014, 11:51:41 pm
content: Quote from: rs20 on August 28, 2014, 11:47:30 amMaking pads smaller may not be a "nasty" thing depending on wether or not you chose your footprint wisely. If you inadvertently chose the M (most) size footprint you may be able to get away with N (nominal) or L (least) depending on how you plan to stuff and solder your board

author: rs20
author_rank: Super Contributor
timestamp: August 29, 2014, 05:53:54 am
content: Quote from: AlfBaz on August 28, 2014, 11:51:41 pmAgreed.

author: ElektroQuark
author_rank: Unknown
timestamp: August 29, 2014, 06:53:40 am
content: Solved reducing solder mask expansion and adjusting the minimum solder mask sliver.I thought that those slivers and mask expansions would form a unity, so the final thickness of mask between pads would be in the safe area, but Altium complained. Maybe I have not a clear view of what is going on.Thank you all.

author: AlfBaz
author_rank: Super Contributor
timestamp: August 30, 2014, 12:37:09 am
content: Quote from: EdoNork on August 29, 2014, 06:53:40 amThis is one area where 3D view is the most help full. Turn off all 3D component models, play around with single layer mode and you can clearly see what's going on with all these values