No solder mask in between footprint landing pads?

Layout
1

Hi!
I’m just about to finalize my first PCB and after uploading it to Oshpark to get a nice visualisation I realised that for some footprints soldermask is not applied in between the landing pads and for some it is.
Of course I could fix this by changing the affected footprints (I didn’t create them by myself) but I’d like to understand if there’s a reason for it and what the consequences would be if I order the board as is. Would the missing mask increase the likelihood of shorts between pads?

Thanks,
Jens

2026×1548 197 KB

1521×910 114 KB

2

Yes. Even if you apply solder paste and subject the PCB to reflow soldering in reflow owen.

3

I fell victim to this on the first board I ever made. Having no soldermask between pads makes it much more difficult to solder boards!

You need to shrink the pad mask clearance (dimensions -> pad mask clearance). You’ll likely have to set it below OSHPark’s minimum clearance, but I’ve had no issues with doing that so far (although it can cause issues).

4

To avoid this ‘mess’ I don’t set the solder mask & paste clearances per pad or footprint (ie. in footprint editor), but only on board level (in pcbnew).
There are rare occurrences where footprints have ‘special’ clearances for special purposes, but they are rare.

5

Thanks for all the valuable feedback! You saved me 30€ plus 3 weeks waiting for an unusable PCB!
So what I did is:

  1. Changed the Pad Mask Clearance globally from 0.2 (default) to 0.1 in --> Dimensions --> Pad Mask Clearance
    This “fixed” all issues besides the ones in the MSOP 10 footprint
  2. For the MSOP 10 footprint I went down to 0.07 pad clearance in the actual footprint