Signal and plane layers

I am using the nightky builds of KiCad6.
Following “How to”-s about plane layers, I can see no diffrence between a plane layer and a signal layer all covered with one zone.

The Gerber for a layer defined as a plane begins by:


A “genuine” plane-layer Gerber would begin like

– etc –

Something I do wrong? Plane layers not fully implemented? I see no thermal relief propeerties in the propeerty box for a pad.

/S Cronatrom

You have seen correctly and you do nothing wrong. KiCad doesn’t have specific plane layers. Do you need in gerbers for some specific reason?

It’s in Properties -> Clearance Overrides and Settings tab.

KiCad V6 does not exist yet.
The closest you can get is KiCad-nightly V5.99.

I also wonder why your Gerber snippet shows V5.1.7 ?

G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.99.0-unknown-9b1890606d~127~ubuntu20.04.1) date 2021-04-22 18:44:56*

You can download the standard for Gerber files directly from Ucamco:

I had a peek through the version I have (X2 Revision 2018.11). It defines at least 14 different "FileFunction** types, but no “Plane”.
(5.6.3, Page 136)

There are also some ambiguities and deprecated stuff in the Gerber file format. It started as a proprietary format from one plotter manufacturer and there have been many dialects in the 40 or so years of it’s existence. Ucamco also has some documents available with guidelines of how to write proper Gerber files.

Actually, I find the Gerber spec rather clear. Here is what it contains about copper layers.

The current KiCad %TF.FileFunction,Copper,L2,Inr*% is valid.
Your “genuine” plane-layer %TF.FileFunction,Plane,L2,Inr*% is not valid Gerber.
Valid would be %TF.FileFunction,Copper,L2,Inr,Plane*%

Why do you need to have Plane/Signal in the Gerber file?

About the second line in the “genuine” example: in section 5.6.4:

Power/ground planes in negative made
sense in the 1970s and 1980s to get around the limitations in the vector photoplotters of that
age but there is no longer any reason for negative today.

Is that example from a gerber file from another, old EDA?

Use of “Negative” is quite common in Gerber files.
Traditionally the solder mask ls an inverted layer.
Here a header of one generated by KiCad:

G04 #@! TF.GenerationSoftware,KiCad,Pcbnew,5.99.0-unknown-99442350a4~142~ubuntu20.04.1*
G04 #@! TF.CreationDate,2021-10-26T22:38:27+02:00*
G04 #@! TF.ProjectId,mumar_base_stm32,6d756d61-725f-4626-9173-655f73746d33,rev?*
G04 #@! TF.SameCoordinates,Original*
G04 #@! TF.FileFunction,Soldermask,Bot*
G04 #@! TF.FilePolarity,Negative*
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.99.0-unknown-99442350a4~142~ubuntu20.04.1) date 2021-10-26 22:38:27*

Apart from negative layers, negative features are also common. It is for example used to subtract pads from silkscreen, and KiCad’s Gerbview has a built-in menu option to make these visible.

I, too, have observed bugs in Gerbv. Gerberlogix is excellent.(

Hi Dindea,

Why do you want to indicate plane/signal on the Gerbers? Or is it that you want to output the planes in negative - then why?

More generally, what is the problem with the way KiCad does things? (It is valid Gerber.)

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