Artefacts in front and back copper layer gerber files

[semo]

Hi community,

recently I plotted my pcb layout and forwarded it to the pcb manufacturer (Würth Electronic). A few hours later I got a call from a service staff that he couldn’t open my front and back copper layer. Silk and mask layers were fine. He told my that the gerber files of these two layers look strange.

Here is an example of the back copper layer output:

%TF.GenerationSoftware,KiCad,Pcbnew,5.1.6-c6e7f7d~86~ubuntu18.04.1*%
%TF.CreationDate,2020-07-01T09:54:32+02:00*%
%TF.ProjectId,driver-board,64726976-6572-42d6-926f-6172642e6b69,rev?%
%TF.SameCoordinates,Original%
%TF.FileFunction,Copper,L2,Bot*%
%TF.FilePolarity,Positive*%
%FSLAX46Y46*%
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.1.6-c6e7f7d~86~ubuntu18.04.1) date 2020-07-01 09:54:32*
%MOMM*%
%LPD*%
G01*
G04 APERTURE LIST*
%TA.AperFunction,Profile*%
%ADD10C,0.050000*%
%TD*%
%TA.AperFunction,ComponentPad*%
%ADD11C,4.700000*%
%TD*%
%TA.AperFunction,ComponentPad*%
%ADD12R,1.600000X1.600000*%
%TD*%
%TA.AperFunction,ComponentPad*%
%ADD13C,1.600000*%
%TD*%
%TA.AperFunction,ComponentPad*%
%ADD14C,4.000000*%
%TD*%

Compared to an old file (which has been produced successfully) it really looks different:

%TF.GenerationSoftware,KiCad,Pcbnew,5.1.4-e60b266~84~ubuntu18.04.1*%
%TF.CreationDate,2019-10-09T10:19:48+02:00*%
%TF.ProjectId,Test_env_J001.1,54657374-5f65-46e7-965f-4a3030312e31,rev?%
%TF.SameCoordinates,Original%
%TF.FileFunction,Copper,L4,Bot*%
%TF.FilePolarity,Positive*%
%FSLAX46Y46*%
G04 Gerber Fmt 4.6, Leading zero omitted, Abs format (unit mm)*
G04 Created by KiCad (PCBNEW 5.1.4-e60b266~84~ubuntu18.04.1) date 2019-10-09 10:19:48*
%MOMM*%
%LPD*%
G04 APERTURE LIST*
%ADD10R,1.727200X1.727200*%
%ADD11O,1.727200X1.727200*%
%ADD12C,0.100000*%
%ADD13C,0.950000*%
%ADD14O,2.000000X1.400000*%
%ADD15C,4.000000*%
%ADD16C,4.700000*%
%ADD17C,2.400000*%
%ADD18C,3.700000*%

I’m pretty sure that I plotted both the same way.

Can anyone tell me where these “%TD*%” and “%TA.AperFunction,ComponentPad*%” artefacts came from?

Cheers
Seb

[der.ule]

Well I haven’t order any PCB with v5.6.1 so far, but I can confirm that for the same project the gerber files plotted with v5.1.6 and v5.1.5 are different, specially at the beginning.

[semo]

Thanks for your reply! It seems that this output format is problematic for the PCB manufacturer.

[kenyapcomau]

I wonder if it’s because you checked the option Use extended X2 format in the plot dialog. I had a fab bounce my job because they couldn’t cope with that. Many manufacturers haven’t adapted to that standard (it has a name, but I’m too lazy to search for it ) so for compatibility when this is option not checked those lines are turned into comments thus:

G04 #@! TF.GenerationSoftware,KiCad,Pcbnew,5.1.5-5.1.5*
G04 #@! TF.CreationDate,2020-06-24T13:55:22+10:00*
G04 #@! TF.ProjectId,zzz,37736567-6d65-46e7-942e-6b696361645f,rev?*
G04 #@! TF.SameCoordinates,Original*
G04 #@! TF.FileFunction,Copper,L2,Bot*
G04 #@! TF.FilePolarity,Positive*

Try Gerbers generated without X2 to see if they will accept them.

[semo]

I’ve tried to plot it also without the extended X2 format but these artefacts still appear in the output gerber file. Also this manufacturer was able to handle gerber files with extended X2 in previous projects.

It seems that there was a change between KiCad’s PCB Layout editor v5.1.6 and v5.1.5 and older versions as @der.ule has also shown.

[kenyapcomau]

Yes but without X2 they are prefixed by G04.

Most of those differences are just the presence or absence of interspersed comments.

Check your fab’s instructions for what standard they accept.

[der.ule]

Where they unable to handle your production files ? (I have no problem opening the gerber files with Gerbv or in OSHPark) Or did just mentioned that they looked funny? As @kenyapcomau mentions, those G04 are suppose to be comments (“G04 Ignore Block Data Y”) and the other change in gerbers in v5.1.6 has to do with G02 syntaxis

https://gitlab.com/kicad/code/kicad/-/issues/3677

[kenyapcomau]

Here’s a previous thread where I ran into a fab not accepting X2.

Pcbway cannot read KiCAD Gerber file [solved]

Hi users. Can anyone tell me if I am doing something wrong. I created a 2 layer PCB, gerbered it then sent the Gerber to pcbway. They say they cannot read it but I used 2 Gerber file readers and both read the file OK. Is this a common problem or am I at fault? Happy New Year to everyone Cheers jeff

As for previous projects maybe another engineer was using a more capable viewer.

[semo]

They where unable to handle my production files, especially the front and back copper layer. For me it’s also possible to open it and review it with Gerbv, which I usually do before sending the data.

Meanwhile I got a call from Würth telling me that the IT has solved it by reconstructing my gerber file without the interspersed comments. But I’m sure that this is just a workaround and next time it will be the same problem.

Okay, I see the difference between using X2 and without.