I have SMD power mosfet footprints from V5 and V6 projects that use an 8 pin package with a power pad.
1, 2 & 3 (source) are drawn connected on the schematic, 4 is gate and 5,6, 7 &8 and also the power pad are drain. Again my symbol draws these as externally connected pins.
Now on V6.99 I get warnings about overlapping pads, this is changed behaviour. Any suggestions how to fix this?
I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
I use one small pad for the gate, one larger rectangular pad for the source, and one largest rectangle for the drain. I guess this does not answer your question, but it works well for hand soldering. I am referring to MOSFET packages such as Infineon PG-TDSON-8 (roughly 5 x 6 mm) or PG-TSDSON-8 (That one is roughly 3 x 3 mm).
Be careful! These Infineon package designations are confusing as heck.
I have boards in production using my footprint, with good yield
I like to follow the manufacturers pin numbering strictly.
This footprint inevitably shorts pads.
Older KiCad versions suppressed the error when the pads were connected on the schematic
You can try and edit the footprint, changing the attribute of the small ‘8’-pads to ‘Heatsink pad’.
Because you have the pads with different numbers (5/6/7/8) instead of all the same number, you need to mark this as a net tie in order to not get warnings (technically you could connect these to different nets in the schematic)
This is the schematic, which worked fine under V5.1 and V6.0
The pins are all connected. I am wary of net-ties as this disables a lot of checking
In 6.99 you can specify which pads are the net tie in the footprint, and it doesn’t disable all checks. Because we added this flexibility, we also added more checks that pins are not allowed to overlap unless they are specified as net tie pins.
Trying the net-tie method, I cannot clear the error
I notice that the symbol and footprint libraries for this package work around by merging 5-8 into one pad 5
This feature is new; @JeffYoung just added it so there may still be bugs.
I was checking that the pad group syntax was correct, so now to raise a report
Raised and quickly accepted by Jeff as a medium priority issue.
Lets see what he finds
It was a good test-case. The main error is that we were using
FindNumberedPad() in the net-tie logic, but it only returns the first pad of the given number.
But there were two other unrelated bugs that it turned up, having to do with how we check netties in zone filling and the router.
In the picture above, the Net Ties section says “Pad groups allowed to short different nets”.
We aren’t shorting different nets but different pads. And the pads are connected to the same net.
I think the description should be changed and if different nets are indeed tied to these pins, that should be an error.
You don’t need a net tie if the pads are on the same net
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.