Soldermask opening on Gerber is wrong and different from 3D

Using the footprint stated below, I experience some strange soldermask opening in the plotted gerbers. The gerbers, PCBNew and 3D viewer is attached for reference. I am looking for errors in solder mask opening configuration, but neither the pads, the footprint or the design is deviation from default (0 in most or all cases).
Kicad version 6.0.1
Footprint: Connector_Molex:Molex_PicoBlade_53398-0571_1x05-1MP_P1.25mm_Vertical
Screenshot for reference:

Is that an online gerber viewer? I try to duplicate the error but in KiCad’s Gerber Viewer it looks like this:

and in Gerbv:

Pretty normal. JLCPCB’s online gerber viewer it known (was known?) for having problems with rounded pads, maybe others do too.

I used this settings to export the gerbers for this quick test:

I just tried the gerber viewer in KiCad (I was using gerbv), in here it all looks fine! So I guess it’s a gerbv issue. Thanks for answering @der.ule

1 Like

Hi, you probably have fallen into this gerber viewer incompatibility bug (not a kicad fault, but viewer): Generate Gerber settings in KiCad 6 - #5 by poco

1 Like

I’d say it’s a user error.
You should never put footprints that close to the edge of a PCB. It probably gets flagged by DRC for this also.

Or are you referring to those yellow quarter circle pie pieces?
Those are not made by KiCad, nor shown in a program part of KiCad.

If you have doubts about Gerber files, then the (online) reference viewer from Ucamco may be a good choice. Ucamco is a company that makes Gerber plotters, and is also the company who develops and maintains the Gerber standard.

Pads with rounded corners are a bit troublesome for lots of Gerber viewers. Gerber files have existed for 40+ years and in those time a lot of dialects and faulty implementations have popped up. Even if your Gerber files themselves are fine, it’s still no guarantee that some cheap PCB shop that uses 15 year old hacked software is going to be able to make it correctly.

About half a year ago, there was some collaboration between someone from JLCPCB and this forum (and/or KiCad developers). Their online viewer also had problems with rounded corners in pads, and they promised to fix their software. I have not kept a close watch on that.

Thanks for your feedback.
Indeed, putting a connector this close to the edge is not wise. It’s a debug connector not for serial production, only hand soldered to prototypes for development. The eastern-most pad I will ask the PCB fab to subtract from outline.

Yes, this is what I’m referring to. I’ve already established this fact, but thanks for your further insight. I’ve been a trusted user of Gerbv for years and never encountered such an issue. Now I know about this one in particular, hopefully I will not encounter another.

There is no need to, you can easily modify it yourself.

  1. Hover over the footprint in KiCad’s PCB Editor.
  2. Depress [Ctrl + e] to load the footprint in the Footprint editor.
  3. Modify that pad of the footprint to your liking.
  4. Put it back on the PCB. (Just close the Footprint Editor, it asks you if you want to save your changes on the PCB.

That is a quick 2 minute solution.
For the full 5 minute solution, it’s better to first copy the footprint into a project specific library, and then also fix the footprint link in the schematic to point to that library. The biggest advantage is that if you reload the footprints from library, then your changes to this footprint are not lost.

But overall, it’s easier and more robust to do it yourself.
What if you forget to talk to your manufacturer for the 5th batch of your PCB’s?

You are certainly right. I like your solution much better, and it’s a good idea to use the project specific library to handle these changes.

Off topic. I do jot understand the purpose to save any project specific library. Here is my workflow: finish the project, release gerbers, zip whole project folder to some kind of release folder.

Next time, you always can unzip pcb and find all custom footprints inside, in case 2nd reversion of the same project is going to happen.

In case one customizes footprint in such a way that it is going to be reused in totally separate project, copy that customized-inside-pcb footprint to your own global library (I am sure everyone has one at least) for future use.

What is the use of project only library?

I can agree with you. If you do a lot of changes to footprints in one board, it should be fine to just do the changes in the layout (2 minute solution). You wouldn’t want these footprints to fill your global libraries. If you plan on re-using the customized footprints, then you should use the global libraries.

But if do a change to the footprint without making new footprint in a library, I wouldn’t trust the changes to always follow the footprint when I update PCB and footprints. It’s a peace of mind thing not to be scared which boxes to tick when updating PCB from schematic.

The main reason for wanting to use project specific libraries for those modified footprints, is that it’s quite easy to reload footprints from the libraries during Eeschema / Tools / Update PCB from Schematic.
During that step it is quite easy to reload the footprints from their libraries (and there is also a specific button in Pcbnew to do so). The result will be that if a modified footprint is only in the PCB, then the changes you made will be lost.

There are different sort of people with different sorts of workflow. some people prefer a structured approach and give value to “theoretical correctness”. Other people have a more ad-hoc approach and fix things only after the damage has been done. I am not sure though which is the best approach. But because I try to be structured and do things “correct”, I presented both methods and let HSPalm decide for himself what suits him best. KiCad accommodates both methods.

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