Platform forum

PowerPak 1212-8 dual - an exotic footprint

robertjzima , 02-27-2018, 10:09 AM
Hello. I'd like to ask your opinion about one special dual Mosfet from Vishay (SI7232DN-T1-GE3) and it's a little bit, exotic footprint. I'm quite scared of designing it in Altium so I came here for an advice. This first picture is recommended footprint by Vishay. It's obvious that every Drain has 2 pad, those from the right side. The problem is, every Drain has also this one big pad that overlaps those two smaller pads but it's not shown as a special pad with it's number. What would be the best practices for this kind of pads?

A) Just create an one big pad for every drain - easiest way .
B) Create special pin for those long pads in schematic and connect it to it's drain. Then do some pad overlapping in altium (I have no idea how).

PS: Those big pads end in the sides of the package and there is no mark with number or anything. What would you do? Thank you very much.
robertferanec , 02-28-2018, 09:07 PM
This may help you how I created similar footprints. Some people may do it differently but I prefer to use simple pads as it is easier for import / export between different CAD systems:

Luca , 03-01-2018, 03:16 AM
I choose the way for this kind of "special footprint" AFTER i've seen also the suggested stencil open.
It's really important aspect like the correct position and dimension of "copper pins" and area.
robertjzima , 03-01-2018, 11:56 AM
Thanks guys! I've chosen Robert's approach. I've created those two big drain pads and added to the schematic also. It looks like this now. Later, I realized one thing. There is gonna be one big polygon for every drain anyway. So the creating very precise and exact footprint is maybe pointless in this case. But I have one more question. Why is there that big difference between solder mask expansion in your footprints? Pad 14 on the second picture has much more than pad 15.
robertferanec, 03-04-2018, 08:11 AM
I do not remember exactly, but pin 14 mask opening may be using the default value which I simply didn't change
Luca , 03-01-2018, 01:25 PM
Tipically the solder mask expansion are suggested from the manufacture of the component, like the stencil opening for the solder paste, don't forget it !
This two aspect concern about the assembly and, in some cases, could be a problem during reflow process and/or Pick and Place assembly.
What i can suggest is to check very carefully the footprint, also about stencil opening, solder mask expansion and copper position.
If the datasheet don't specify stencil opening and/or mask espansion try to ask to manufacturer for some kind of information or documents.
Could be also very usefull check the gerber files of "demo" board, if they exists.
I hope this can help.
robertjzima , 03-01-2018, 02:09 PM
Thanks! I was trying to find those numbers but there is no sign about solder mask a paste expansion in the documentation. I found some separate documents from manufacturer about the footprints they use in general, but this didn't help. There were only information about soldering process, temperature etc... I'm gonna try again or maybe I can ask manufacturer as you recommended.
Luca , 03-01-2018, 02:32 PM
We are happy if you find some help in our answer!
Another important aspect that i consider when i create a footprint is about the basic rotation of the component.
I try to respect the orientation of the component like manufacturer says that is positioned inside the reel.
This could be helpfull for the assembly house during the assembly process because the PP file that you generate with Altium
report the correct rotation for the component.
Regards, Luca
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?