Hi,
My PCBA told me that the solder mask must be removed between the pads of a SOT1268 (DFN1412-6) device, but I can’t find the correct way of doing so.
Setting the Solder Mask to copper clearance to 0.22mm didn’t change anything.
Keepout areas don’t work with solder masks.
Tweaking the footprint by adding a solder mask rectangle covering it entirely makes the design rules checker generatye 38 errors.
What did I miss ? Thanks.
If the DRC error was solder mask aperture bridges items with different nets, this it really wasn’t an error in this case, was it?
Not really an error, and I could ignore it. However, I don’t want to tweak every footprint a la DFN / QFN. Rather, I would like to know what parameter(s) should be changed so that all such devices have the solder mask removed under them (or at least between all pads).
Then, you probably want to change the Soler mask minimum web width to a value large enough to account for the space between pads.
(Which will also generate the same DRC error.)
Edit: I realize I didn’t allow bridged solder mask apertures between pads. After putting the solder mask min web width to 0.3mm, I got the purple under the device as expected. The 3D viewer is buggy and still shows plain solder mask around pads, but the Gerber viewer shows the right thing. Thanks !
PS: and no DRC error 
I am surprised the value you use.
I had (since 90s) used 3 mils as mask expansion and also 3 mils as minimum web width. Manufacturer didn’t questioned it. Later when he got to have www home page I found that he assumes that standard is 4 mils for both these values. Since 2017 (I use KiCad) I have these both values set to 0.075mm. But recently after arrangements with manufacturer in some cases I use even smaller values: mask expansion down to 0.065mm and minimum web width down to 0.07mm. So I can have mask strap in 0.2mm gap between pads (2x0.065+0.07=0.2).
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
