making multi pined footprints where pins are the same function

[Simon]

I have created a footprint for a part. It is a PG-TSDSON-8 footprint, basically a lead less package with 4 pads, but on one side the 4 pads are independent and on the other side the 4 pads are all the drain of the mosfet. I could not see how to number each pin and include the big thermal pad in the middle without making the 4 separate pads and then put a pad number "0" in the middle to join them just like the footprint drawing showed. Except now the design rules don't like these 4 pins that are all on the same net being joined like this. Maybe the answer was to make all the pads the same number?

[ahbushnell]

I would make the the same number

Sent from my SM-G930V using Tapatalk

[T3sl4co1l]

Sometimes the datasheet specifies the pins as individual, and elsewhere specifies which pins are tied together internally (usually by listing the pins beside the respective terminals in the circuit diagram, or putting terminals and pins in a table to the same effect).

How you go from here to there, in any particular EDA tool, is up to you.

Some allow you to assign multiple footprint pins to a given schematic pin.  Multisim is such a tool; Altium/CS is not.

If you cannot, then you can solve it any other way you like.

I like to make this specific footprint by numbering the pads according to the schematic symbol (which itself might be numbered based on something else, like the SPICE model if applicable).  All pads of a given name will be placed in the same net (and won't have collision errors), so all the shapes which make up the drain pad are numbered the same.

The footprint isn't very reusable this way, but it isn't very reusable anyway, on account of the huge pad shorting everything together.  There might be some devices that use pins 1-4 independently, but who cares, and if you need to use one you can just make a variant of the footprint for it and be done.

Alternately, you can number pads individually, and enumerate all the pins on the schematic.  This makes for ugly symbols, but is the most specific (the schematic tells you that this part has lots of pins, and that they're all connected together externally and internally).

Tim

[Simon]

Thing is all of these pins are connected on the schematic. I'll do a MOSFET only version using G, D, S instead of numbers. I expect all MOSFETs in this package are the same.

[jmarkwolf]

I must preface the following with the fact that I commonly do the things below in Altium Designer, and have not yet done them in Circuit Studio, but I expect they will work just as readily in Circuit Studio.

Yes, itemizing all the part pins of a schematic symbol does clutter the schematic a little bit, but it is un-ambiguous and you won't have to dig up the datasheet for "clarification" in the future. I like to think of the schematic as the "gospel", unless of course you're trying to obscure the real intent of a design, which can be a strategy as well.

I also like to reserve any pad numer "0" for features such as mounting holes in a DB15 connector for instance. If such a pin is not represented in the schematic, or simply not connected, then it will be left out of the netlist.

When parts have big thermal slugs underneath (I call them "bare bellies"), I'll give them a pin on the sch symbol, even if the part doesn't have such a pin (for clarification). The VNH5019 part below has only 30 "real" pins but I identified the three "bare bellies" with their own pin numbers 31, 32 & 33 and "described" them on the schematic symbol (for clarification). I even broke these pads out into multiple individual pads with voids between them for solder paste gas escapement, which can sometimes "blow out" the solder reflow from underneath the part, causing loss of flow for good thermal conduction. Very important for parts that "run warm". Doing it this way also gives me extra versatility in connecting the part on the PCB.

[Simon]

Well is CS from what I can tell I can't make random pad shapes but can agregate simpler shapes.