Footprint AOZ226

[maykol_rey]

hello, some chip designers let their imagination run wild and create chips like the AOZ226X from alpha and omega.

So far so good, but how do I trace that… the “big pads” are in contact with the small pads and this doesn’t allow me to connect.

Any recommendations on how I should handle this type of footprint?

footprint downloaded from Digikey
QFN4X4-22L_EP2_S_AOS.kicad_mod (12.5 KB)

[mf_ibfeew]

If I should guess I would say the big inner copper areas are only copper-rectangles, not proper pads. So I think the footprint is false designed.

But to get a reliable answer: add the project to your thread (or as a minimum at least the footprint).

[maykol_rey]

I already added the footprint, eset downloaded it from digikey

[mf_ibfeew]

I guessed right (what have I won?). The big inner copper areas are simple filled polygones and therefore independent copper.

You have to correct this false footprint.

I would recommed to start drawing that footprint from scratch - that needs more time, but it’s the best way to learn this. You could first make a copy of the original footprint and than work on that copy. So nothing bad can happen.

For drawing the custom pad shapes I have copied one of my older answers:

• all connected copper-areas must be defined as one pad, so pads 7+8+9 must all renamed to pad7 (and 10+11 to 10)
• click & select the normal pad which should serve as the anchor for your custom pad shape (one of the pad7-pads)
• RMB-click → context menu–>Edit pad as graphic shape
• footprint-editor canvas changes into “pad edit mode” (see yellow warning bar at top of screen)
• now draw all custom copper-items onto the central pad. All copper-items which connect to that pad form later the custom pad shape.
• It’s enough if a copper-item connects to the anchor pad through another copper-item, a direct connection to the pad is not necessary
• you can use any copper-shape (line, circle, arc, rectangle, polygone unfilled or filled)
• If you are finished with your custom form: RMB-click–>context-menu–> Finish pad edit mode

note: if you modify this footprint you have to (most probably) also modify the symbol in the schematic - as the correct footprint doesn’t have pins 8+9+11 anymore.

@gkeeth : could this enumeration be copied into the kicad-pcb-docu (as starting-point for section " Creating and editing footprints → Custom pad shapes")?

[BobZ]

I have been designing power electronics for many years, although I am not familiar with this IC. I did download a datasheet.

Your first 10 priorities are to follow the layout recommendations in the manufacturer datasheet:

Many switching regulators can have unexpected malfunctions if the layout is imperfect. There are interactions that are difficult to predict.

It seems to me that pins 21 and 22 have a gap between them according to the datasheet. For some reason I do not see this gap in the 3d image at the top of this post. Making footprints in KiCad is not so difficult. Be sure to observe the footprint drawing in the datasheet. Double or triple check to avoid errors.

[gkeeth]

@mf_ibfeew

@gkeeth : could this enumeration be copied into the kicad-pcb-docu (as starting-point for section " Creating and editing footprints → Custom pad shapes")?

I’ll take a look, can’t promise it will be soon though.

[davidsrsb]

@mf_ibfeew

all connected copper-areas must be defined as one pad, so pads 7+8+9 must all renamed to pad7 (and 10+11 to 10)

KiCad now allows pads to be defined to be shorting, an improvemnt on the old net-tie kludge

[mf_ibfeew]

The original digikey-footprint was a good example why I don’t like downloaded footprints. Only exception if I get the footprint recommended from someone I thrust (edit after a hint: I trust him.).

• the main fault: bad, non-working pad definition
• more slight niggles (but nevertheless valid):
• misleading footprint name (in fact it’s a QFN24 with 2 pins missing)
• no pin 1 marker on silkscreen
• instead some curious extra rectangles on silkscreen without obvious reason
• reference string placed on top of central pad
• no description string
• fabrication drawing with way to thin lines - gives barely readable printout
• courtyard: lines to thick (distracting on board view during routing) and unnecessary complicated (such things slowdown the drc on really complicated boards)
• courtyard: to small defined - does not reserve space for pick&place machine to the next component

a slightly repaired footprint:
QFN-24-2EP_4x4mm_AOZ2261.kicad_mod (7.7 KB)

This version also implements the idea from aris-kimi and davidsrsb: connected pins are correctly defined and than assigned to net tie groups. This feature is new in v7, so here is a picture:

This new feature looks nice and overcomes my first proposal to rename 7+8+9 pads all to pad 7.

caution before using this footprint:

• I have not checked the geometric dimensions of the pads
• I have not checked how the footprint works with the corressponding symbol
• I personally would reduce the paste-area for the two big exposed pads - but this depends on manufacturer. Sadly there is no recommendation in the datasheet.
• I have not checked if the new “net-tie”-solution for pads 7+8+9 (and 10+11) really works in schematic-board

[eelik]

@mf_ibfeew

Only exception if I get the footprint recommended from someone I thrust.

If someone recommends you a footprint you thrust him?