MSOP-10 pads are too long

Layout Footprints
1

The pads for the MSOP-10 package are too long.


Housings_SSOP:MSOP-10-3x3mm_Pitch0.5mm

904×560 33 KB

Suggested pad layout from Linear Technology data sheet

This causes board assembly problems at this fine pitch. There’s only 0.195mm distance between pins. Because there’s pad under the raised part of the pin, solder migrates there, and can form solder bridges. Those can’t be removed easily, because they’re under the raised pin area.

Is that a bad footprint? A footprint for a different class of part? Or what?

(Version info: Version: 4.0.6-e0-6349~53~ubuntu16.04.1 release build)

1 Like
2

Hi,

You may want another footprint for this part: MSOP-10-1EP_3x3mm_Pitch0.5mm

3

It does not look like he needs an exposed pad.

4

I guess this footprint has been designed with extra long pins. We can not check it because the pdf link given in the footprint is dead.

I would suggest you open an issue over at the github repo. Or better still correct the footprint and open a pull request.

5

You’re right, Rene.

But the exposed pad can be removed and the pad sizes of the other 10 pads are the same he is looking for.

Anyway, sometimes I followed the vendor’s footprint guidelines and then the manufacturer asked me for a little longer pads.

1 Like
6

  1. It’s really that the pads are closer together across the width of the device than they should be. Extra length in the direction away from the device isn’t a problem. The data sheet calls out a 3.20mm to 3.45mm separation, but the footprint is 3.00. (That doesn’t seem like much, but it’s enough to allow solder bridges under the raised part of the pins. Very frustrating rework session under a microscope today. Do not want to do that again.)

  2. Are the MSOP footprints drawn manually, or is there some generator that cranks out footprints for different numbers of pins? In other words, is there some generic place to fix this, or does it have to be fixed on a per-footprint basis?

  3. A keep-out area in the footprint to prevent the autorouter from attaching to the pins from underneath the chip would be nice. Attachment from the wrong side is troublesome at this scale. It exposes a tiny bit of extra copper under the raised part of the pin. Feature first requested in 2012.. Was that ever implemented? It’s not just an autorouter problem; it’s also a problem with copper pours.

7

I think the current footprints are hand drawn. (The clue is that all of them look different.)

You can create a generator with the scripts by @pointhi (I think this would be the best solution in the long run.)

You can add a keepout are in pcb_new but there is no way to define it in the footprint.

1 Like
8

Unfortunately an answered question, not a wishlist item, so effectively closed.

9

I made up a project-specific footprint which matches the LT3750 data sheet specs. Available if anyone wants it.