[SOLVED] Edit solder paste layer or stencil aperture

Is there a way to divide the aperture into 4-6 parts in a layer of paste using kicad? This is very important for qfn to 220 cases where there is a large cutout for heat dissipation . By default, the paste file generates one large square and there are no editing tools for gerber kicad …

do not pay attention to the size of the footprint, you are only interested in dividing the central part for an example
On the left is what the kicad generates, on the right is what you need to get .

See how it is done in for example:


this is the problem that i don’t understand how to do it in kicad… using my footprint i expect that it is possible to change the solder paste layer… then generate the desired gerber… or change the stencil gerber itself…

If the central pad also specifies a similar sized solder paste area . . .

. . . then you need to untick the F.Paste layer and make your own as desired . . . remember a custom footprint need to go in a custom library.

1 Like

The footprint I shown is from KiCad library. Just play some time with it to find how it is done.

Thanks for the hint, everything worked out) but it’s hard to understand the logic after exporting the board from Altium) The first thing I encountered was the different assignment of layers during import, everything has to be edited manually, the silkscreen is gone, plus, as you said, you still need to add components from the board to your library))) while in the opposite direction, when you need to transfer the board to altium, everything is fine…

1 Like

While on the paste layer, is there a command for a negative value to draw a polygon? Place Region ?

I don’t understand the question.

for example in altium it is done like this

Decrease the size of the automatically generated paste feature to zero (by making the paste mask expansion a negative number).

Then add whatever shapes you want to the paste mask layer using the Place Region command.
Do kicad have something similar?

To create the mask/paste objects you could (in kicad):

  • enable/disable the automatic shape generation for every pad
  • if enabled: use the pad-shape plus/minus a modifying value (pad/footprint properties–>clearance overrides page), this creates a enhanced/reduced shape
  • you could always place nearly any graphic object you want on the paste/mask layer. You like a triangle - draw a 3-point polygone. Eception: it’s not allowed to place rectangular circles.
  • Last option is to place SMD aperture pads - these aare pads without copper (and without net), but only with paste/mask layer.

The resulting paste/mask is the sum of all these objects.

Even if you have already plenty of experience with a different cad I second the recommendation of @Piotr : play with existing footprints/symbols/designs and try to look how the standard delivered symbols/footprints/design examples are made. Most settings are done with the properties dialogs for the items - so it’s important to learn which setting is located on which properties-dialog sub-page.

1 Like

:+1: Thanks
Thanks for the answer… Another small question… If I leave a negative gap, then in this place the solder paste layer is not generated… But when checking the rules, kicad does not indicate an error, similarly with altium… Is it possible to include in the check negative clearance?

Now I got what you mean.
When using for that purpose a negative number you may be used to use for example -100 mils always and once for a bigger pad you can forget that this time you have to write -200 or bigger negative.

In KiCad it is simpler. If you want to not have paste opening generated for the pad you simply uncheck the right checkbox without having to think if your negative number is enough big.

For me using the negative number here is like using a side-effect of something, while using the check-box is informing the program exactly what is your intention. It is also faster in implementation when program based on one bit knows that shape need not to be calculated then after making calculations for all 4 pad sides (and may be for rounded corners and may be for other complex pad shape) it have to found that resulting shape not exists.

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