Footprint Design: SolderPaste Layer Problem


I am still working on my VSON Footprint. @SchrodingersGat has noticed, that some of the solder paste layers are missing. I am sitting here for an hour or two to find a solution.

First problem -> marked as 1

On Pad 1 the solder paste layer is active…

and only the solder mask clearance is set (specification from the datasheet)

No Solderpaste on pad 1 :confused:

Second problem -> marked as 2

The Solderpaste Layer is to small. It must be the same size as the pad.

There are no Restrictions. The only restictions on the size of the solderpaste layer are on the middle four pads.

Is there a global setting that i am missing?

Thx for help :wink:


That appears to me to be the Legacy Canvas; which does not appear to show the stencil dimensions (solder paste layer).

Change to Open GL canvas; under the “View” menu drop down, or simply depress F11.

Then select the “working layer”, on the right menu bar “F.Paste” with a mouse click.


hm, i am still in OpenGL mode. The solderpaste layer is there on the other pads. You can see it in the 3D screenshot.


Well, this was an issue that I was curious about. The #2 “pad” you have circled is NOT a pad. It IS the solder paste/stencil outline. There are in fact 8 small stencil openings for the ONE large “H” shaped pad.

The other markings around the other “pads” such as shown in the circled #1 pad is the solder mask.


The 3D viewer solderpaste clearance is being derived from the current setting in PCBnew… no matter what you set it in the footprint editor.
If you’re working in OpenGL you can see it in the editor itself though (with the real settings for the pads).

Looking at the clearance of the pads where the paste shows up, it tells me that the pin pads 1-12 are too small for the current clearance from PCBnew to cause visible paste in the 3D viewer for that footprint.

Change the setting in PCBnew to ZERO and see what happens.

IMHO, please be aware that it is bad practice to define paste mask clearances and solder mask clearances in the footprints, unless you know what you’re doing


This statement is not exactly correct. The stencil opening setting for each footprint determines the amount 2D dimensions of total solder that will be applied to the pad, and the 3D thickness of the stencil will determine the final entire volume.

Take a look here:

Yellow/Goldish plated COPPER PADs.
Neon Green Annoyingly visual SOLDER PASTE.

The resistor footprint specifies the SOLDER PASTE to be “exactly” the same size as the COPPER PADs; in the 3D viewer, this makes the COPPER PADs not visible. .

In the image, the part on the right, requires less solder to be applied to the COPPER PADs and all three items can be clearly seen.


Ok, i got the error. I don’t know if ist is a bug and can’t build it again. I opened the footprint in a Editor a found at the top of the data this lines…

(module Texas_S-PDSO-N12 (layer F.Cu) (tedit 58D1493A)
  (tags "SON thermal pads")
  (solder_mask_margin 0.05) <--
  (solder_paste_margin -0.1) <--

solder_mask_margin and solder_paste_margin are set as global. Change both to 0 fixed the Problem.

Anyhow, i don’t know, how i have done this. :slight_smile: Now all is fine … again…


Hm, thanks for the feedback. Will have to look at this I guess and check it out again. Changed behavior then. :+1:


Hey Joan, just to let you know, the colors the OP used, and the text of the problem, threw me off a bit.

And, this statement by me is CORRECT, "[quote=“Sprig, post:4, topic:5979”]
The #2 “pad” you have circled is NOT a pad. It IS the solder paste/stencil outline. There are in fact 8 small stencil openings for the ONE large “H” shaped pad.

Which I have now learned is how KiCad deals with odd stencil/solder paste issues on large/complex shapes footprint for re-flow oven soldering.

To the OP, now that you have SIGNIFICANTLY INCREASED the solder paste on the “H” shaped pad, you might want to double check the data-sheet for suggested values if you are going to try to put this board into production.


Hi Sprig,

the full covered legs of the H-Shape is the recommendation for this footprint. Also the 0.05mm Solder Mask clearance on the pads 1 to 12 are the recommendation.

But thx for the hint, i will try the footprint soon and give feedback.