Hello,
I’m trying to design the footprint according following land patern.
My solution was to add a F.Cu rectangle over the pads:
But when i try to route the track from pins 29-40, it gives me the error: Cannot route the track from a graphics.
What is the best aproach how to do that properly?
Kicad v 5.99
Thank you,
Hynek
Copper zones are not “graphics”.
Even if you put graphics on a copper layer, it still is “just graphics”.
You can’t assign a net name to graphics for example.
You can’t use copper zones in the footprint either.
The normal way to handle this in KiCad is to use a lot of overlapping pads, and give all the pads the same pad number. There are plenty of examples of this in KiCad’s libraries. Just search for any footprint with the string “ThermalVias” in it.
You can also add graphical shapes to a pad. To do this first select a pad, then right click on it and select: Edit pad as graphic shapes.
There are also special “aperture pads”. These are pads which do not have copper at all. These can for example be used to make a cutout in the soldermask
We can also give some more options if you give a direct link to the datasheet of the component. For example, are those pins always connected, are they connected internally, is it possible that some pin is left unconnected and a track covered with soldermask going under it (not of course recommended, but could be possible)?
If the pins always serve the same purpose and are always connected like that, it would be possible to simplify the symbol by having only one pin which has for example number “29…40” and create only one pad which also has the number “29…40”. The pin number is actually just text, so this is possible. Then each solder mask opening should be an unnumbered “aperture pad” as Paul said.
Thank you for your comments.
The part is LMG3422R050. Land pattern is on page 34.
https://www.ti.com/lit/ds/symlink/lmg3425r050.pdf
These pins are Source and Drain. I did solve this by “Edit pad as graphic shape”, which is not ideal as visible on pin 15.
But if the pad name is just text as @eelik suggested, this seems to be ideal solution. In this case, it will also solve my issue with hidden pins in symbol (I do overlap all source and drain pins with “passive” type).
This solution has only one big disadvantage for me. Custom Mask and Paste needs to be created as Rectangles, right? Pads have their origins in the center (same as in datasheet), but for rectangles, i need to define coordinates for starting and end point, which is very annoying.
Sorry but I came from different CAD and I’m just learning.
Thank you,
Hynek
Sorry guys, i completely ignored the “aperture pad” solution 
Everything is then solved, thank you.
Hynek
I was a bit confused by this statement.
Then realized it refers to the “29…40” text string.
Pin “numbers” are indeed alphanumeric strings, but they do have a limit of 4 characters (Oops. This limit is apparently lifted in KiCad-nightly V5.99).
This sure is a weird part / footprint.
It needs some thought. Both of how you want it to look like in the schematic, and for how to connect copper to it on the PCB.
The example on page 23 of the datasheet looks quite horrible:
One way is to use “pin stacking”, but then you still have to define all the pins in the schematic symbol, and this does not look very useful in this case. Working with aperture pads does seem a much more logical choice.
All the Drain pins (1 through 16) are quite close to the thermal pad on the bottom and this is connected to the Source (Page 3). In KiCad all track ends have rounded ends, and this won’t fit, so drawing a copper zone is your only option here.
Pads with rounded corners are good practice, but you made your pad rectangular. It’s better to define pads (or better: solder stencil layer) with rounded corners. First, it’s not feasible to have real sharp corners in the solder stencil itself, and second, rounded corners release the solder paste better. (This is also noted in note 6 on page 36 of the datasheet).
The datasheet has a clear example suggestion for both the Solder mask layer and for the Solder Paste layer. Not much to add here, except that I won’t use (most of) the pin numbers in KiCad myself. (Although it’s logical that each pad has a number in the datasheet).
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
