4
\$\begingroup\$

I generated a 4x4mm 0.45mm pitch QFN28 according to the Atmega328P datasheet:

enter image description here

However, the pads on the corners (1+28, 21+22, 14+15, 7+8) are too close to each other, less than 0.2mm apart (when datasheet says the pins are 0.4mm apart because of the chamfer).

The solution that comes to mind is to make the pads on the corner shorter, as I did with pads 1 and 28:

enter image description here

Which gives about 0.3mm clearance:

enter image description here

Is this the proper way to do it? If I just leave the pattern as generated I will most likely get DRC errors depending on the process I pick (0.15mm vs 0.2mm).

I know the assistant is just a tool and not set in stone, but I'd just like some informed answers about the proposed solution. (Or alternatives)

Update after answers:

Thanks to DerStrom8 for the App note. Here follows a comparison of IPC generated and Atmel/Microchip recommended patterns:

Left is Atmel/Microchip App note (~0.266mm), Right is IPC wizard from Altium (~1.77mm)

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ facepalm, maybe I picked "Least" when generating the footprint... \$\endgroup\$
    – Wesley Lee
    Feb 4, 2019 at 13:15
  • \$\begingroup\$ I would just camfer the IPC decal corner pads to achieve the wanted clearance. The pad doesn't need to be oval shaped. \$\endgroup\$
    – TemeV
    Feb 4, 2019 at 15:31

3 Answers 3

Reset to default
3
\$\begingroup\$

Unless you're etching this yourself, a clearance of 0.2 mm probably won't be a problem for the manufacturer. 0.127 mm (5 mil) is not uncommon, and 0.152 mm (6 mil) is even more common. I would check your board house's requirements and modify the DRC rules to match what they are expecting. Then if there are any specific issues based on your manufacturer's rules, you can focus on them one-by-one.

If you want to bypass the IPC footprint altogether, you can go with the recommended land pattern from Microchip/Atmel themselves. See page #12 in this app note: http://ww1.microchip.com/downloads/en/appnotes/atmel-8826-seeprom-pcb-mounting-guidelines-surface-mount-packages-applicationnote.pdf

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ Ah I didn't even think of looking for their own footprints, for some reason I never find Atmel footprints. I changed the pads on the land pattern to compare the clearances, will update it on the answer. \$\endgroup\$
    – Wesley Lee
    Feb 4, 2019 at 13:09
  • \$\begingroup\$ Yeah, some companies store their land patterns in a separate document or documents, so it takes a little extra work to find them. \$\endgroup\$
    – DerStrom8
    Feb 4, 2019 at 13:27
2
\$\begingroup\$

The drawing in the datasheet is the actual package itself, not the pad layout you have on the board. The PCB pads will be slightly larger than the package pads to allow for slightly imprecise placement. This will be corrected by surface tension when the solder is in the molten phase. The PCB shape generated by the IPC wizard will be fine (as long as it meets your manufacturer's DRC minimums).

\$\endgroup\$
2
  • \$\begingroup\$ Yes, I know its the package, the thing is the IPC wizard generated a footprint from those dimensions, which would force me to go with a more expensive process. So basically I am asking if my modification is acceptable to avoid needing a more expensive process just due a couple of pads. Thanks for the answer. \$\endgroup\$
    – Wesley Lee
    Feb 4, 2019 at 12:59
  • 1
    \$\begingroup\$ @WesleyLee As long as the PCB footprint is larger than the package's pad, you should be fine. I'm surprised that manufacters can't do QFN as minimum, but there you go :) \$\endgroup\$
    – awjlogan
    Feb 4, 2019 at 13:09
2
\$\begingroup\$

I created custom pad shapes (one cut on the right, one on the left), and then replaced the eight corner pins on the package.

  1. I started with an IPC-7351B-compliant package created by Library Expert.

  2. For the new pads, I started with the dimensions of the IPC-7351b-recommended oval pad, and then manually modified them to create the chamfered corners. I calc'd the chamfer dimensions to end up with my required clearance between pins on the completed package.

  3. Finally, I went to the symbol itself and replaced the 8 pins in question with my new pad shapes.

This was using Cadence OrCAD.

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.