Hi KiCaders,
Does anyone have experience with SMD footprints containing Pads which are different than Stencil apertures?
Specifically, I need to design LGA package with huge pads (2x2mm) which contain 4 smaller stencil aperture window, and thus do not open the whole Pad area.
By default, Stencil aperture is the same shape as Pad area, with specific size offset - that’s easy.
But how should I design other shapes for my stencil? Should I use ordinary graphics polygons on the Solderpaste layer and arrange them as I want? Or is there a better approach?
yes
.and twenty more
With KiCad it is very common to combine multiple pads with the same pad number, to make complicated pads. This is used extensively for SMD IC’s with thermal pads for example.
In a similar way, you can also use one pad for the copper layer, and another pad for the stencil aperture.
Have a look at some of the footprints ink KiCad’s default libraries.
Open the Footprint Editor, then enter “thermal” in the search box.
An example of a footprint where some pads only have F.Paste layer is:
Package_FN_QFN / QFN-24-1EP_5x5mm_P0.65mm_EP3.4x3.4mm_ThermalVias
[Edit]
Eeliks’ addition is a good one. I can confirm that the pads on F.Paste do not have a pad number set.
1 Like
In the footprint editor create “aperture pads” without a pad number. Tick off the paste layer in the main copper pad properties.
You should not add graphics for this purpose on the board paste layers.
And the aperture pads must not have a pad number.
1 Like
Thanks 
I will try to win my fight 
EDIT:
Just tested - and it works. Pad type “SMD Aperture” did the trick.
Funny thing is, if I select Pad type to SMD Aperture I can create my Stencil “Pads”, but after I Edit the stencil pad, they restore to ordinary “SMD”. I’m on 5.1.7, wonder if that’s intentional.
EDIT2:
It’s a bug. Reported as issue # 5036 , fixed for Master but not cherrypicked to 5.1.x
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.