KiCad stackups contain wrong prepreg thicknesses when multiple prepregs without copper are present

[schweigstill]

KiCad doesn't support stackups with multiple prepregs without copper between them. Altium Designer doesn't have this problem. E.g. jlcpcb_8L_1.6mm_outer1oz_inner1oz_JLC081611-2116.kicad_pcb contains the following definitions:

		(layer "In2.Cu"
			(type "copper")
			(thickness 0.03)
		)
		(layer "dielectric 3"
			(type "prepreg")
			(color "FR4 natural")
			(thickness 0.109)
			(material "Nan Ya Plastics NP-155F 2116")
			(epsilon_r 4.16)
			(loss_tangent 0.02)
		)
		(layer "dielectric 4"
			(type "prepreg")
			(color "FR4 natural")
			(thickness 0.109)
			(material "Nan Ya Plastics NP-155F 2116")
			(epsilon_r 4.16)
			(loss_tangent 0.02)
		)
		(layer "In3.Cu"
			(type "copper")
			(thickness 0.03)
		)

"dielectric 4" will be skipped during import of the stackup, so the total thickness isn't calculated properly.

KiCad's behaviour is well documented, this is not a KiCad bug. Possibly future versions will allow sequences of multiple non-copper layers.

Tested with KiCad 9.0.0, release build.

[schweigstill]

I just noticed that it is even worse: the non-copper layers get shiftet, which leads to an asymmetrical stackup.

[gsuberland]

Thanks for the report. This should be pretty easy to fix by combining the alike dielectric layers together. I'll take a look at the code and make some changes.