What does "No solder mask between pins" mean? - Page 1
Forum section: electronics / general

author: zphaze
author_rank: Contributor
timestamp: May 01, 2020, 10:58:23 am
content: Hi,I did a PCB recently with Altium and used a footprint from the internet that, from my perspective, should be fine.Anyway, the PCB I did got reviewed by someone from the company and one of the points mentionned wasthat "there is no solder mask between the PINs of this IC"I'm showing a preview of the footprint of the said IC :I'm not sure I understand what this means, hence why I'm asking!Thanks

author: maxpayne
author_rank: Regular Contributor
timestamp: May 01, 2020, 12:27:10 pm
content: Make the solder mask exception in all those pad properties to 0.05The one you have now is the default

author: zphaze
author_rank: Contributor
timestamp: May 01, 2020, 12:30:02 pm
content: I'm a bit newbie with Altium.I'm still not sure what this is all about.First, I'm not even sure what the purple around the pins is.I never really bothered to be honest.I thought this was a non conductive layer already?

author: pigrew
author_rank: Frequent Contributor
timestamp: May 01, 2020, 02:01:42 pm
content: The purple is the solder mask layer. It's a "negative mask" meaning that the mask will be removed from where the purple is (it needs to be removed from the pads, so you can solder there.The solder mask helps prevent solder bridges between pins during assembly. Usually one needs a "solder mask sliver" of at least 4mil (and often more) in order for it to be reproduced reliably by the PCB fab. Fabs may (and often do) expand or contract the mask layer during data preparation, generally trying to end up with the layout that you designed.When you have the solder mask set properly, there will be an individual rectangle of purple around each pad, with a non-purple region between the pads.PS: When I saw your title, I figured that you would be one of my students at university. I just mentioned this issue to a good number of them.

author: zphaze
author_rank: Contributor
timestamp: May 02, 2020, 05:28:04 am
content: Thanks for these very useful informations.But I wonder, if I now want to adjust the solder mask expansion for this particular footprint, what value should I use?For the record I would like to use JLCPCB (their capabilities are listed here :https://jlcpcb.com/capabilities/Capabilities)Are the infos on this page sufficient to deduce what I can use?maxpayne says 0.05, is that a common value for this kind of pitch or..?

author: maxpayne
author_rank: Regular Contributor
timestamp: May 02, 2020, 05:32:30 am
content: you can check the datasheet of the IC and see if there is any suggested value from the manufacturer. If not there you may check the manufacturer footprint guideline also.If not .05 just works fine.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: May 02, 2020, 08:22:11 am
content: For 0.50mm pitch, I use 0.23 to 0.25mm width pads, 0.076mm expansion (from rule), and 0.094mm minimum soldermask sliver (also called "web width" elsewhere). Most fabs can do this standard.The hazard is that, without mask between pads, there is a greater risk of bridges/shorts forming.Refer to IPC-7351 for footprint calculations. Should be able to find an old copy online somewhere.Tim