Hey guys, I am quite a newbie in KiCad and i am trying to model an exposed metalic pad on top of a ADC encapsulated component. According to the datasheet of my component, there is a pad on top of the encapsulate that should be connected to ground (EP). If you’re curious i am using the DAC from Maxim MAX1184. How can i model that exposed pad and draw a connection to ground, so it appears like that in the final layout?
Thanks in advance guys!!
The exposed pad is on the bottom of the IC and it connects to a pad on the PCB.
Okey that´s something to take into account for the PCB layout!. But anyway i guess i have to indicate that is there somewhere in the schematic. How can i do that?
On the schematic you just add another pin to the symbol, pin 49. Then you can connect it or mark it as unconnected according to the datasheet.
@1.21Gigawatts mentioned one approach:
[quote=“1.21Gigawatts, post:4, topic:4615, full:true”]
On the schematic you just add another pin to the symbol, pin 49. Then you can connect it or mark it as unconnected according to the datasheet. [/quote]
This creates an additional pin on the schematic symbol, which may confuse somebody who knows how many “normal” pins the IC package has. And, to avoid ERC squawks, the additional pin needs to have a connection shown in the schematic or the “not connected” symbol attached. Some folks call this “visual clutter” and claim it’s confusing.
Another approach exploits one of KiCAD’s VERY useful features: Overlapping pads WITH THE SAME PIN NUMBER are merged into a single piece of copper. This lets you build up pads with complicated outline shapes, using rectangles, circles, ovals, etc, as basic elements.
To do this, add a pad to the footprint, positioned where the thermal pad sits. Give it the exact same pin number as one of the GND pins (pin 13, or pin 16 look like good choices). Then define yet another “pad” (with that same pad number) to make the electrical connection between the thermal pad and the actual GND pin. The footprint examples in my posts at More via on a pad and How to add via holes on a thermal pad of QFN footprint? and also Pad Holes Under SMT for Heat Sinking and other questions are a starting point, although they do not include the pad functioning as an electrical jumper.
Dale
For a part that has the equivalent of an additional pin, requiring a footprint that has an additional pad.
The pin is usually named something like “EP” which shouldn’t confuse anyone who knows the part.
As for which which method is more or less confusing is purely subjective. But despite your detailed explanation and links to examples I’m sure the OP will still have questions.
OK, so I looked closely at the links I posted and realize they don’t agree very closely with what I tried to describe with words.
Here’s another version of the SSOP footprint, with the thermal pad electrically connected to a GND pin in the footprint. The associated schematic symbol will have only 20 pins, not 21. Before you use this footprint for ANYTHING EXCEPT AN LTC4011, make sure that pin 5 is the ground pin!
LTC4011_SSOP20_Pitch0_65mm_ThermalPad_Handsolder_GNDconn.kicad_mod (4.8 KB)
Dale
thank you very much for your feedback!!