Mask cutouts for pads are combined at gerber export

hi, a footprint (F-mask layer) seems ok as below pic 1.
But it became a Block pattern after gerber (pls check pic 2).
Can someone offer an advice to help?
Kicad 5.1.0 Mac version

I assume you show the soldermask layer. KiCad merges nearby cutouts if the clearance between them is smaller than your minimum soldermask width setting. ( Sadly this is only done on gerber export. A known issue.)

This is necessary to ensure that your manufacturer is able to reliably produce your board. (Assuming you setup the rules to fit their capabilities. )

1 Like

Great thank!
Solve it till I set solder mask min width as 0.05mm.
Need to ask if fab can produce it.

thanks again

0.1 or 0.15 mm would be more probable minimum.

1 Like

Oh. the device is DFN 2x2mm and its recommended footprint is as below.
I follow the recommended design, the smallest width in F-mask layer is 0.06mm.
Please advice how to adjust the layout~

For some opinions see Make sure you read all the posts and then decide if you still want to have smaller minimum width.

1 Like

That suggested footprint seems extremely strange to me. IPC suggests at least 0.2mm clearance between the center pad and outside pads. (The graphics style of the drawing further decreases my confidence that this is made by somebody competent to be honest. The lack of tolerances is another clear indication that somebody might not have been qualified for the job they did.)

1 Like

I’m stuck!
Even I leave 0.2mm at space, still ERROR after gerber in F-mask layer?
Or it’s NORMAL?
(I set solder mask min width as 0.1mm)

Any advice?

The features on your solder mask layer look fatter than the copper layer. What is your solder mask clearance? If it is greater than 0.05mm then you are asking for less than your minimum 0.1mm between the center pad and the outside pads.

Depending on your manufacturer’s mask clearance minimum (sometimes called pull-back) and minimum mask width, you may not be able to get any mask on such a small footprint.


you are right.

I think there is a separate setting for “solder mask expansion” somewhere…

In KiCad V5.1 there is:

Pcbnew / File / Board setup … / Design Rules / Solder Mask / Paste

With my default setup, all 4 values are set to zero.
Apparently you can also enter negative values to make solder mask holes smaller than the pads.

SMD pads may also have separate settings for solder mask, and may be set to overrule the default setings. To check this, you can click on a pad and then press “e” for edit and then select the “Local Clearance and Settings” tab.

Not only single pads, but also Footprints have settings for solder mask and solder clearance. I do not know how all these settings interact with each other.

1 Like

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.