Gerber Solder Mask Output 20x bigger in 5.02 vs 4.06

Layout
1

Hi,

I recently migrated the hermeslite SDR design from 4.06 to 5.02. When I plot the final gerber files, the solder mask files are 20x larger due to a reduced APERTURE list. In 4.06 I had the long apertures list shown below but in 5.02 there is only one aperture. Although everything still looks correct in gerber viewers, the files are much larger and more importantly, I can not apply post-processing scripts based on specific apertures. Is this a bug, and if not, is there any way to enable the old behavior?

Thanks,

Steve

Single aperture in 5.02:

G04 APERTURE LIST*
%ADD10C,0.100000*%
G04 APERTURE END LIST*

Multiple apertures in 4.06:

G04 APERTURE LIST*
%ADD10C,0.100000*%
%ADD11C,1.000000*%
%ADD12R,1.343000X0.835000*%
%ADD13R,2.050000X2.050000*%
%ADD14C,2.050000*%
%ADD15R,0.835000X1.343000*%
%ADD16R,1.550000X0.600000*%
%ADD17R,1.597000X1.089000*%
%ADD18R,2.600000X5.900000*%
%ADD19R,1.800000X2.000000*%
%ADD20R,1.089000X1.597000*%
%ADD21R,2.500000X5.800000*%
%ADD22R,1.200000X0.600000*%
%ADD23R,1.400000X1.600000*%
%ADD24R,1.200000X1.200000*%
%ADD25R,1.978000X2.994000*%
%ADD26C,1.600000*%
%ADD27C,2.000000*%
%ADD28C,3.450000*%
%ADD29C,2.740000*%
%ADD30R,1.000000X1.100000*%
%ADD31R,1.100000X1.000000*%
%ADD32R,2.000000X1.800000*%
%ADD33R,1.600000X0.500000*%
%ADD34R,0.800000X1.250000*%
%ADD35C,5.500000*%
%ADD36R,1.850000X2.740000*%
%ADD37R,1.215000X1.850000*%
%ADD38R,0.960000X1.850000*%
%ADD39R,1.850000X2.200000*%
%ADD40C,2.300000*%
%ADD41C,2.800000*%
%ADD42C,3.000000*%
%ADD43R,2.740000X1.850000*%
%ADD44R,1.850000X1.215000*%
%ADD45R,1.600000X1.400000*%
%ADD46R,1.280000X1.240000*%
%ADD47R,2.140000X2.150000*%
%ADD48R,1.200760X0.799440*%
%ADD49R,5.200000X1.800000*%
%ADD50R,5.200000X3.500000*%
%ADD51R,1.300000X1.800000*%
%ADD52R,1.250000X2.400000*%
%ADD53R,2.400000X1.250000*%
%ADD54C,3.200000*%
%ADD55C,2.400000*%
%ADD56C,1.400000*%
%ADD57C,2.250000*%
%ADD58R,1.200000X2.710000*%
%ADD59C,0.700000*%
%ADD60R,12.200000X2.400000*%
%ADD61R,1.100000X1.450000*%
%ADD62O,0.900000X1.600000*%
%ADD63R,2.200000X5.000000*%
%ADD64R,1.200000X4.200000*%
%ADD65R,0.900000X1.600000*%
%ADD66R,2.100000X4.480000*%
%ADD67R,2.700000X2.700000*%
%ADD68R,0.450000X1.000000*%
%ADD69R,1.000000X0.450000*%
%ADD70R,7.200000X7.200000*%
%ADD71R,3.000000X3.000000*%
%ADD72O,1.400000X0.480000*%
%ADD73O,0.480000X1.400000*%
%ADD74R,5.200000X5.200000*%
%ADD75R,0.710000X1.300000*%
%ADD76R,3.700000X2.800000*%
%ADD77R,1.700000X0.850000*%
%ADD78R,2.900000X3.800000*%
%ADD79R,0.800000X2.400000*%
%ADD80R,7.200000X3.140000*%
%ADD81C,0.700000*%
%ADD82C,0.700000*%
%ADD83C,0.000000*%
%ADD84C,0.000000*%
%ADD85C,0.254000*%
G04 APERTURE END LIST*

2

Pads using rounded rectangles for a start lead to much bigger, but still correct Gerber files

2 Likes
3

To answer my own question, PCBNEW will revert to the old behavior of creating multiple apertures if “Solder mask min width:” is set to 0. This can be changed via the GUI menu, Setup->Pads to Mask Clearance… But when I change this value to 0 to match my 4.06 project and save the 5.02 project, this value does not stick. When I reopen the project, the value has always reverted to 0.25. This strikes me as a bug. I always have to set to 0 before generating gerber masks.

Thanks,

Steve

1 Like
4

Is it possible that your pads are too close together to generate mask in between them for your selected mask clearance and solder mask min width combination?

I would suggest to take out a calculator and check if 5.0.2 removes mask here correctly or if 4.0.6 was right in keeping it. (Depending on the outcome either of them has a bug but only bugs for 5.x.x will be addressed.)

5

In 5.02 the Solder mask min width is set to 0.25mm when opening a V4 project
this has been fixed in nightly/5.1 so the soldermask min width will be 0.0 when converting

1 Like
6

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