PCB Libraries Forum : Solder Mask On 0.40 Pitch QFN https://www.PCBLibraries.com/forum/ Wed, 15 Apr 2026 18:10:09 +0000 Fri, 27 May 2022 14:10:32 +0000 http://blogs.law.harvard.edu/tech/rss Web Wiz Forums 12.07 360 https://www.PCBLibraries.com/forum/RSS_post_feed.asp?TID=3127 <![CDATA[PCB Libraries Forum]]> https://www.PCBLibraries.com/forum/forum_images/PCBLForumLogo.gif https://www.PCBLibraries.com/forum/ <![CDATA[Solder Mask On 0.40 Pitch QFN : You could simply make the solder...]]> https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12451.html#12451 Author: feynman
Subject: 3127
Posted: 27 May 2022 at 2:10pm

You could simply make the solder mask openings 1:1 land size and leave the manufacturer the option for resizing according to their capabilities (in your fabrication notes).

The big question here is if 50 um of solder mask clearance is enough for your manufacturer's capabilities. You should definitely ask them about that. Try being as specific as possible when you ask ("Can you leave solder mask between the pads of THIS footprint or will you gang mask it?").

If they say they can do this you might want to explicitly call out in your final data to not gang mask, nevertheless. Because sometimes manufacturers can, but don't want to :)

If they need more clearance than 50 um for the solder mask they will very likely Gang Mask it like Tom said.

]]> Fri, 27 May 2022 14:10:32 +0000 https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12451.html#12451 <![CDATA[Solder Mask On 0.40 Pitch QFN : The Fabrication shop will automatically...]]> https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12438.html#12438 Author: Tom H
Subject: 3127
Posted: 25 May 2022 at 9:34am

The Fabrication shop will automatically Gang Mask the entire row of pads on all 0.40 mm pitch packages. 

]]> Wed, 25 May 2022 09:34:25 +0000 https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12438.html#12438 <![CDATA[Solder Mask On 0.40 Pitch QFN : Hello,I am working on a footprint...]]> https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12437.html#12437 Author: ArtCym
Subject: 3127
Posted: 25 May 2022 at 4:59am

Hello,

I am working on a footprint for a QFN package (component MPN is ICM-20948) which has 0.4mm pitch and I'm not sure how to design the solder mask for this footprint. 

I saw some examples online where for QFNs of 400um pitch it was advised to use solder mask trench around the pads since it might be hard for the manufacturer to place solder mask between pads (minimum webbing of 100um in my case). 

Still, I would like to have solder mask between pads to help avoid solder bridges and I thought that I could use the nominal lead width instead of the maximum lead width to use for my footprint. 

I will use 50um solder mask clearance in my design. My idea is to use the nominal pad width (200um) + 2x50um of solder mask clearance leaving me with 100um for the solder mask webbing.

My question is if it is too risky to use the nominal width of 200um instead of the maximum 250um but have the benefit of solder mask between pads?

]]> Wed, 25 May 2022 04:59:03 +0000 https://www.PCBLibraries.com/forum/solder-mask-on-0-40-pitch-qfn_topic3127_post12437.html#12437