I have a very high density footprint with 70 pins that has different pad and mask shapes. I’m hoping there is a way to make a pin have a different mask shape than pin shape so that I don’t have to manually create each mask. I’ve also thought about diving in and writing a python script (though I know python and have modified the BOM scripts I’m worried that its a rabbit hole that may take more time than drawing 70 masks shapes with rounded corners. Any suggestions about how to approach this footprint?
Scripting doesn’t seem to work in the footprint editor (but it looks like you can make a script to generate a new footprint). I was hoping to just find all the existing pins and add a mask and paste or the correct size in the same location.
I can copy and paste an individual pin and the change it so a SMD Aperture with rounded corners.
Create an aperture pad, then right click on it and Create from Selection / Create Array.
And its indeed also possible to use a scripted approach to generate a footprint. There are about 15 of these footprint generators in Footprint Editor / File / Create Footprint. These are python scripts, so you can use one of them as a starting point to create your own.
You can also make only one then Right Mouse click select Duplicate (Ctrl + D hotkey) and if you set your grid correctly after making the original, they should land in the right place when moving.
Or, create one pad, then right click on it and select Copy Pad Properties to Default and then just start adding pads with those properties.
You can also:
First draw the normal pads.
Set the grid to something coarse (20mm) or so. (beware of grid offset).
Duplicate your existing pads and move them a few grid points.
Change one of the duplicated pads and Copy Pad Properties to Default.
Select all the duplicated pads, right click and Paste Default Pad properties to Selected
Move these modified aperture pads so they fit again over the other pads.
And there are probably more methods too. KiCad has quite a lot of ways to avoid or simplify repetitive tasks to speed them up. Spending some time to learn to use that will be well worth it in the long term.
I’m happy to ignore a few errors but because these connectors have so many connections and I have two connectors built like this I have 140+ errors that I have to wade through to find real issues.
First, you have two apertures in one aperture pad: Mask and Paste. The “metal mask opening” is the Paste aperture, at least that’s how I interpret it because the paste stencil is metal while the solder mask has nothing to do with metal. You should have only “Paste” ticked in your aperture pads. The copper pad should have Mask ticked but not Paste.
The error message means that there are two different items belonging to two different nets under one mask opening. The mask opening doesn’t of course have any net. I don’t know why this happens here. Try to fix your pads as I explained, maybe that helps.
If not, How does solder mask layer work? may give an answer. Maybe the mask bridges/webs/dams are removed and KiCad v7 handles it as an error? If so, IMO it’s a bug because a large mask opening is expected to bridge items in that case. At least one mask opening should give only one error.
@eelik Thanks your your response. I think I have a pretty solid understanding on soldermask / paste. If you look at my first message the requirement from the part manufacturer is that the mask is smaller than the pad. I just discovered that I can adjust the "Solder mask expansion by a negative number but this doesn’t get me to the manufactures recommended shape (since the shrinkage is not uniform in the x and y as well as it has rounded corners).
At this point I’m going to live with the errors and hope that someone comes up with a better suggestion before I send the final board out. But yeah, this connector might be an interesting edge case for improving the footprint / pad tool.
I still believe the “metal mask” is the metal stencil for the paste. I don’t see why they would recommend using solder mask defined pads, especially with different shape than the copper.
In any case you should have only one layer in these aperture pads.
This is normal and expected.
Aperture masks do not have pin numbers, and they also do not need them because there is no electrical connection.
That is called a Solder Mask Defined Pad, you’ll find lots of references when you paste that magic string into the Wonderfully Weird World.
I also believe you are staying too close to the “manufacturers recommendation”. If you have a solder mask defined pad, then it really does not matter much how much copper is under that pad. The most important parameter is that the (negative) “solder mask expansion” is bigger then the maximum misalignment that your PCB manufacturer specifies between those layers. Therefore, I would just start with having a look about misalignment tolerances for a few PCB manufacturers, take the biggest tolerance and add some more just to be sure, and then calculate the pad size from the aperture cutout and the solder mask expansion.
Having rounded corners in apertures is good. Sharp (inner) corners are impossible to make, and also solder paste tends to stick more in sharp (-er) corners. Therefore rounded corners in pads improve process repeatability and reliability. But nobody cares how much copper there is on the pad under the solder mask, and just using a rounded rectangle for the copper itself is just fine.
A problem you will bump into is that PCB manurefacturers do weird things with your design. It is very common they add their own margins, and this can wreak havoc with your design if you’re not careful. So be sure to communicate this with your PCB manufacturer.
How much effort is really put in such recommendations by the manufacturers?
Is it an recommendation from a 20 year old datasheet? If the datasheet is recent, has that recommendation been revised, or just copied from the 20 year old datasheet?
I don’t like sloppy work, but I do not consider giving some thoughts about “recommendations” found in some datasheet a bit of consideration instead of treating them as the holy grail.
Ah, I see what your saying. Thanks for hitting me in the head a bit more more so that I am more willing to see what you are getting at. I’m a little snow blind because I’m trying to get my webbing up to .2 mm (PCB Way Capabilities for green mask) so that I have a mask between pads. I may have to go without webbing.
(a task for tomorrow).
