Create differents sizes for BGA footprints


I can create differents sizes for the solder pad, solder mask and the silkscreen ?

I can create pad n1 with 0,28mm (round) for the solder pad F.Paste
Pad n1 0,38mm for the solder mask F.Mask
and pad n1 0,34 for the laser silkscreen 0,34mm F.Silk

It’s ok for the LPC55S69JEV98K?

Best regards

Simply make pads with just the layer you want it to have. Any pad without copper should then get an empty pad number.

Pad on silk? what would be the use of that? Is it possible you confused layers here?

Thank you

For this

The picture looks like a solderpaste stencil. This is typically defined with the paste layer that you already list. Might it be that one of the layers should be copper? (Possibly link to the datasheet of your component)

There is also an alternative to adding one pad per layer. You could calculate the required clearances for past and mask relative to the copper size. This would reduce the workload for you as you only need to set a single value per layer in the footprint settings.

We also have a script that could help

The recommended sizes are in pages117,118 and 119

In the datasheet:
Copper, F.Cu, “solderable area” (at least I understand so): 0.28
Solder mask opening, F.Mask: 0.38
Solder paste stencil opening (made with laser in thin metal plate), F.Paste: 0.34
No silkscreen (F.Silk) in specs, it has different purpose.

See What is the meaning of the layers in pcb_new and in the footprint editor?.

You can define the copper pad as in the specs and set the mask and paste clearance to proper values to make up the final specified values in the pad properties.

1 Like

Yes, it’s so, thank you, sorry the confussion.

I can create a pad for each kind and called 1 to all.

For create the array it’s easy, I know it.

They suggest soldermask defined pads with the following diameters:

  • F.Cu 0.38mm
  • F.Mask 0.28mm
  • F.Paste 0.34mm

This can be made with the following pads and footprint settings:
All pads get the size of 0.38mm and have F.Cu, F.Paste and F.Mask enabled.
In the footprint settings set soldermask clearance to -0.05mm (yes negative number) and paste clearance to -0.02mm (leave pad clearance and paste ratio clearance alone)

1 Like

Rene, how did you find that mask/copper values? I think the “solder mask opening pattern” page has clearly 0.38mm diameter for the mask opening.

I have done this:

F.Cu 0.28mm
F.Paste and F.Mask enabled.

Solder mask clearance --> 0.1mm (positive)
Solder paste clearance --> 0.06mm (positive)

I’m waiting for Rene’s answer, I may have misunderstood the datasheet. Meanwhile, those clearance values should be halved - it’s that value in all sides of the pad and becomes double when measuring the final diameter. Just measure each layer in the footprint editor after setting the values.

This is the footprint, now I have that remove the leftover pads.

VFBGA-98_7.0x7.0mm_P0.5mm.kicad_mod (24.1 KB)

VFBGA-98_7.0x7.0mm_P0.5mm.kicad_mod (14.6 KB)

I confused mask and copper. (misremembered between reading the datasheet and writing it down)

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