|T O P I C R E V I E W
||Posted - 08 Sep 2021 : 14:12:23
Is it possible to add different footprints to a part using the same symbol but with different pin assignment?
To be more concrete, I am trying to add a single part which is a mosfet pair, with contains 2 mosfet transistors in a single package. I want to add two different footprint TSOT26 and SOT563. The problem is that the pin assignment varies in each package, for instance, in the first footprint the gate of the first mosfet is the pin 1 while in the second the pin 1 is the source, but I can only have one gate mapping per schematic.
Is there anyway to achieve this behavior?
|3 L A T E S T R E P L I E S (Newest First)
||Posted - 08 Sep 2021 : 22:49:53
This example is for a dual-gate FET FDC6312P, which may be similar to your requirement for one of your parts. In this case use the pin names:
G1 S1 D1 for Gate, Source and Drain on the first gate;
G2 S2 D2 for Gate, Source and Drain on the second gate.
Just use the same pin names on the second part with the other footprint.
Download Attachment: FDC6312P_example.zip
||Posted - 08 Sep 2021 : 21:39:16
This example is for two of the MSP430FG4616 family that has either a BGA or QFP footprint. There are two parts with two different footprints, but one symbol, and Pin naming, such that the device can be changed on a circuit diagram from one part to another easily without making a mess of the schematic diagram connections.
Download Attachment: MSP430FG4616_BGA&QFP_example.zip
||Posted - 08 Sep 2021 : 21:29:09
Yes, it's quite easy to do, though you will need the two different parts to be actual different parts with different footprints.
I do this myself with all diodes, FETs, BJT transistors so I can swap between parts that have different pin mappings and footprints.
Here's how I do it with a couple of example components.
Diodes, where you have some diode parts using SOD two-pin packages and some using three-pin SOT-23 packages.
Have one schematic symbol, using Pin 1 and Pin 2, making Pin 1 the cathode end and pin 2 the Anode end.
In your SOD footprint, also have pin 1 the cathode and pin 2 the anode.
In your SOT-23 footprint, have your pin number 1 to 3 the normal way.
Create a part for your SOD diode using the footprint and symbol that you've created but in the Part Editor click the tab at the bottom named "Pins". You'll find it between the tabs "Parts and Attributes" and "Gates".
You will see the left-most column called Footprint Pin. In the column immediately to the right called "Pin Name" change the Pin Name over to something sensible.
I use A for Anode and K for Cathode.
Then in the Gates tab you match up the symbol pin to the footprint as normal.
If you use Logic names on your symbol then this process, using A and K provides an extra sanity check to ensure your devices are all the right way around!
Next, in your SOT-23 part, do the same thing and enter the Pin Name relevent to the function of the pin, again using A and K. Ignore the third pin - keep it as a number.
In the Gates tab for your SOT-23 part, again, match up the footprint pin to the schematic pin.
Now when you insert either of these parts in your circuit diagram you can swap between the different parts when you want, with your schematic diagram remaining connected correctly, since it's using pin numbers K and A for both parts.
For BJT transistors just use the pin naming B, C, E for Base, Collector, Emitter
(that's why I use K for the cathode of diodes, so I use C for the collector of BJT transistors)
For FETs just use S, D, G for Source, Drain, Gate.
If you have a device that uses both a BGA package and a QFN it is still possible to do the same thing.
I have done this for some MSP430 devices by using pin names in the fashion: 1/A2 where 1 would be the pin number 1 of the QFN or QFP and A2 would be the datasheet footprint pin A2 of the BGA.