[SOLVED] "Broken Ring" pattern in paste layer for footprint generation


The above looks to work now, but as a general comment, the exact details of the paste-ends, probably do not matter much, as the paste melts and reflows anyway.
I would not fret too much over rounded ends.


Heh… do you mean the user is stress-testing the application, or the application is stressing the user?

I think the fundamental issue here is that I am not at all familiar with the CAD part of the process. I do have FreeCAD but I’ve only used it for importing/exporting files really. I tried a fresh approach this morning to create a simple sketch and how to constain it - then FreeCAD crashed on me, twice. At that point I decided to leave it for a rainy day…

As for my actual footprint - I decided to just use arcs a long time ago. But it annoys the hell out of me when I don’t understand something, especially something that looks as powerful & useful as this.

@maui - do you have any example Freecad file saved anywhere that I or anyone else could try?

Also, I have a small bug to report: I was exporting to a temporary footprint on my desktop and overwriting every time I tried something. When I use the KiCAD export button to save a footprint then select the existing file I get the “Are you sure?” prompt then “File saved to…”. But it doesn’t actually overwrite the file! I was trying different things but loading the same old file into KiCAD :frowning:

This is Win10 x64 and a fresh install of KiCAD 5.0.0 and FreeCAD 0.17.


the file is included in the demo and can be reached through StepUp Demo menu (see the picture above)


  • latest StepUp
  • FC 0.17 + (fine from stable to dev release)


Where were you trying to export the footprint to? Windows won’t let you save to a system folder, for example anywhere in Program Files. I think in this case it might actually save it elsewhere and not let you know, but I forget where.

Also, if you were trying to save your export into the KiCad supplied libraries, DON’T for another reason. The next time you update KiCad the installer will happily overwrite your changes.


Doh! I didn’t notice the menu right in front of my eyes!

Anyways, that’s perfect, just what I needed. The example imported just fine and gave me a working baseline to start with. It looks like my sketch was broken - I used Sketcher to make a simple outline (basically one of the segments) and it worked OK.

Not sure what the naming conventions mean yet “Pads_Polyxxx” etc, but that’s sure to be a case of RTFM which I can do at leisure. Right now it’s a sunny day and my wife is reminding me I have a house to paint… :smiley:

Thanks for your help & patience!

PS ref the save location - just my desktop which is definitely write-able. I think it may be the fact that something was wrong with the file causing the export to not happen.


If you need help regarding the sketcher, i found a tutorial in the freecad forum:
https://forum.freecadweb.org/download/file.php?id=64732&sid=b487beb523c271f4322e17c947a3a409 (This is a work in progress.)

The discussion thread is found here: https://forum.freecadweb.org/viewtopic.php?f=36&t=30104 (If the file is updated, the new one will appear at that place)


I managed to implement also the recently added primitive geometry (only ‘circle’ and ‘polyline’ are supported atm).
Please update your KSU tools.
I updated also the FC demo model…

and here the result in KiCAD


Looks good! Actually I managed to create my footprint after a few days messing about with FreeCAD. I didn’t get on too well with the Sketcher UI which seemed [to me] to be doing strange things so I just used the macro facility then edited the macro with the values I needed to get the arcs / lines right. Then it was a pretty simple task to export it to a module.

The mic in question was a Knowles SPU0410LR5H, the footprint I made is attached.SPU0410LR5H.kicad_mod (3.4 KB)


Hi @nali
I would suggest you to remove BackCu (selecting Layers to F.Cu) and BackMask (unchecking B.Mask) from the PAD #6 of the footprint… then you will have a full SMD fp as in the data sheet.


Hi @maui

Thanks for the comment. I did ponder whether to make a B.Cu pad, and decided to include it after all. The footprint is SMD, but because it is a bottom-port type microphone a hole is needed anyway, so I thought I might as well include the bottom pad. It’s a GND connection, so I use it to connect to a B.Cu flood fill.

(In reality nothing will be mounted in this area on the underside of the PCB because it normally fits against whatever case the board is mounted in for sound entry.)


I can actually think of a good reason for not allowing that hole to be a PTH. You don’t have to worry about solder getting in the hole and blocking it during manufacture. The solder on the component side around the hole might have a tendency to wick down a plated hole, especially if there is slightly too much solder paste.


+1 … and some chars


I’m not following that - the solder paste area is a long way from the hole ?
What may be an issue is solder mask ink getting into the hole - a NPTH hole avoids that, but if it is the only NPTH hole, that will cost more.
Careful tune of PADSTACK sizes to avoid both solder and mask-ink issues, should find a PTH solution ?


But it isn’t on the footprint that @nali posted. The 3D view up above is @maui’s example. Here is what @nali’s design looks like (front and back) in the 3D viewer:

Though, I suppose a better question to @nali is why his design deviates so much from the originally posted image. Round pads where there should be square, two extra pads, size of the pad around the microphone hole (the OD of your pad is 1.224mm, but the drawing specifies 1.45), pin numbering doesn’t match, etc. Did you upload the right model?

Well, that depends on the manufacturer. More and more board houses now don’t charge extra for NPTH holes.

I don’t know why not having asked them, but I suspect that they expect everyone to have NPTH holes. Thus NPTH holes would already be built into the cost of the board, even if the board design doesn’t use them. For all I know may they have the routing bits and NPTH drill bits all on the same turret and do the routing and NPTH drilling all in one CNC job (probably in the other order, holes then routing…). Similarly, per via pricing seems to have also vanished from the industry.


Oops, yes, I just glanced at maui’s images, and had not spotted the large differences to earlier images…


I used a model from a general DS of SiSonic, not knowing the real user case adopted, @nali redesigned it to his model

The drill should be NPTH with a less drill size


here a second release :wink:

SPU0410LR5H-r2.kicad_mod (3.8 KB)
PS I’m not sure about the pin numbers… in the DS it is not clear if the view is from top or bottom


Ah. He didn’t provide a link to the actual datasheet when he finally mentioned exactly what part he wants to use, and I didn’t bother to go find it.

Ain’t communications fun? :stuck_out_tongue_winking_eye:


My target was to introduce him to the use of generating footprint in a mechanical environment, plus improve my tools :wink:


Quite simply my OP was about how to generate the segmented ring, and the image was a Google Images search for such a pattern. I deliberately didn’t attach or link to the specific part because I wanted to find out how the process works rather than hope that somebody just comes up with my footprint (or give the impression that’s what I wanted).

I certainly wasn’t expecting @maui to add it to his demo!

I must admit I hadn’t considered solder migrating down the hole so I’ll probably tweak my footprint a bit. Knowles’ design guide isn’t much help in this respect, about all they offer is

The solder stencil pattern must be optimized for production, and for bottomport SiSonic models must use a broken solder ring such as that shown in the figure below