Relatively new to KiCad. I’m trying to create a footprint for a TO-263-7 Regulator. I’d like to include pads for the heatsink as part of the footprint, but there are some unusual things about this that I’m not sure of.
Below is the footprint opened in editor, followed by 3D view.
Q1. Ground is on pin 4. Can I label the other thermal pads also as pin 4 as I’ve done? Will this match up correctly with a schematic symbol that only has 7 pins?
The large pad to the left in the first picture is the size of the drain pad, but isn’t part of the solder mask layer. I moved it to the left for visibility in this picture only. However, when I place that pad over the top of everything else, it just looks like a giant single pad. No matter what view I check or uncheck, it looks like a standard pad. However, opening within 3D viewer it looks normal.
Q2. Is there a proper way to view solder mask layers within the footprint editor? Or is it not intended to be used like this at all?
Yes this does indeed work. In fact having multiple pads with the same number is the only way to create complicated pads in kicad. (If two pads with the same pin number overlap, kicad notices that they are already connected which could come in handy if you want a more complicated pad than a simple rectangle.)
In open gl mode you can switch to the pad outline view. This way everything is much easier to see.
The solder mask layers don’t show the solder mask that is automatically generated over the footprints. In fact, these solder mask openings usually don’t have a definite size until the footprint is placed into a board layout, where the “Solder mask clearance” and “Solder mask min width” parameters are defined. (See the drop-down menu “Dimensions” > “Pads Mask Clearance” in PCBNew.) Yes, you CAN over-ride these settings with specific values in the footprint editor but that is the exception rather than the normal procedure.
For better or worse, the Gerber files are the de facto method of communication between the board designer and the fabricator. Occasionally there will be an error due to a buggy Gerber interpreter but this is actually rather rare. It is the Gerber files, not the 3-D models, that you should use as the standard for what features will, or will not, appear on each layer. By overlaying various combinations of Gerber files in a Gerber viewer you can get accurate measurements of things like clearance, overlap, spacing, etc.
There are several threads on this Forum dealing with footprints for devices that have thermal pads. (E.g., TO-220, SOT-223, DPAk, etc) I provided links to some of these discussions in my post at Modeling exposed pads on top of encapsulate
Thanks for the quick and concise answer. It seems this is the most suitable way, and this helped me.
But you are still defining areas, with selections for ‘with’ or ‘without’ solder mask. Clearance is applied to those defined areas on the footprint. Again, the areas themselves still exist, and you should be able to view these areas.
I guess I was expecting to be able to check/uncheck visibility on the layers and see differences between pads that have solder mask and pads that do not. It doesn’t appear to actually do that within footprint editor.
[quote=“dchisholm, post:3, topic:6645, full:true”]
It is the Gerber files, not the 3-D models, that you should use as the standard for what features will, or will not, appear on each layer.[/quote]
The 3D model was an easy example of proving that the pad settings were actually working, since the footprint viewer gave no indication. Why does the 3D viewer have layer capabilities that the footprint viewer does not?
Of course the gerber file is the last thing I’d look at for a full board, but I’m not used to checking a gerber file for each new individual footprint I create. Is that what you are suggesting?
By design, KiCAD doesn’t behave that way. This behavior is either a “charming eccentricity” for those who don’t want the visual clutter of seeing a mask cutout over every pad; or an “annoying quirk” for those who’d like to see every design detail displayed at each step of the design.
And, as I tried to point out above, the mask openings aren’t even precisely defined until the footprint is placed within a board design.
[quote]. . . Of course the gerber file is the last thing I’d look at for a full board, but I’m not used to checking a gerber file for each new individual footprint I create. Is that what you are suggesting?
[/quote]
I have never done a specific test layout for a newly-created footprint, but I believe some designers do exactly that. Usually when I create or modify a footprint, I have a target PCB layout close at hand and I can verify the new footprint in the exact layout I created it for. It probably sounds a little condescending (or perhaps even arrogant) but my accumulated experience with KiCAD and other layout programs gives me the skill and confidence to know how a footprint change will manifest itself on a board layout. As the old admonition says, “Practice, practice, and practice!”
(And, for the record, before I submit a set of Gerber files to a fabricator I sit down with my coffee and a trusted Gerber viewer and carefully inspect every square centimeter of the board, displaying each layer and combinations of layers, measuring things like clearance, setback, annulus, etc. With KiCAD it is especially important to look at the silkscreens, since they are completely ignored by the DRC algorithms.)
