so8-diodes-inc.zip (10.1 KB)
Hi,
I made a SO-8 to suit Diodes Inc chips. The default SO-8 footprint is way off. I don’t have time to tidy and push to git so anyone who’s up to it feel free to take ownership.
Regards,
Andrew
I haven’t examined your footprint, but I hope it includes some explanations of its differences from the default SO-8 footprint. It is possible that Diodes Inc produces an SO-8 package which is not in compliance with industry standards and requires a different footprint, but it’s more likely that the company-supplied footprint was created with different assumptions than the default footprint.
Whenever I find myself re-inventing somebody’s wheel I always wonder if I have rounded off all of the corners . . . and whether there was a reason the other guy left some corners on his design.
Dale
You’d have to ask Diodes Inc that one, but for brevity C1, Y and X are smaller. X could be left as is but Diodes Inc recommends a slightly smaller size. The pitch is the same, perhaps it is this which defines the SO-8 “standard”.
As Diodes Inc chips are popular it’s very much worthwhile getting this into the library. I only caught it after prototype.
The footprint I attached needs the reference name removing, I’ve never understood why Kicad saves that instead of a placeholder.
Just looking around, Vishay use another SO-8 spec, so they’re all different.
Rather than use the manufacturer should be able to differentiate in the library using 1.27 (pitch) and the C1 value.
Did you follow the link in the datasheet? The one you are looking at is 2013, the referenced one is 2017. Which is dimension K?
The pad layouts in datasheets are often just suggestions, there is rarely anything unique about them. Even if they have followed an IPC standard, IPC provide for several variants. So really take the suggested layout with a pinch of salt.
Note in the case of SO-8, there are wide and narrow versions. “SO-8” sounds like an old KiCad footprint, recent ones have dimensions specified in the part name to avoid confusion.
1 Like
Hi Bob,
The SO-8 footprint in kicad is way off, the pads only just touch the pins and I mean just.
K = X, my fault sorry adjusted.
The SO-8 in the library does have the dimensions, I initially took it (as a newcomer to PCB design) to be a standard (as there was only one). Sticking another in the library (this one I hope) will avoid that confusion.
Regards, Andrew
If that is the case then the most likely reason is that you are confusing the wide and narrow variants of the SOIC-8 package.
1 Like
Hmm, ok so if you pick a footprint with the wrong dimensions, it will have the wrong dimensions. 
There are short form descriptions like “SO-8”, but there are usually several variations, for example, wide/narrow. There is also naming differences, like SO, SOIC, SOIJ which are similar but essentially synonymous. The actual difference may be package height, which is not important for PCB layout.
KiCad has a sample of popular variants, but is not comprehensive. In any case you need to select one that matches the dimensions of your part, or is close to. In this case, probably SOIC-8_3.9x4.9mm_P1.27mm, and there is no need to add a new variant.
2 Likes
You can find variations even in the same brand, due to different package and test facilities
OK - SOIC-8_3.9x4.9mm_P1.27mm is the one.
… which Diodes Inc call SO-8.
I’ll put more emphasis on measuring everything from now on.
A good way to check footprints is by using FreeCad. (This is how we check the footprints for the official lib.)
I wrote up a tutorial on that.
1 Like
While you did remove your initial statement it seems you might be, or were, a little confused regarding the terminology. SOIC refers to a particular package family of which there are several variants. There is a wide body variant (7.5mm) and a narrow body variant (3.9mm). And to make matters even more confusing, there is also the less common medium body variant (5.28mm). The dimensions listed are body widths, not lead or pad dimensions.
Edit: And yes, SO is often used as a short form of SOIC which can also add to the confusion. Glad to see the Kicad libraries are now using the full name.
Edit: And according to IPC there is also an extra wide body variant (9.02mm).
1 Like
Going forward I think when you select a footprint Kicad should create a preview which includes the basic measurements between the pins. This can then be directly referenced in whichever datasheet is being used and prevents the ambiguity.
If only reading the datasheet was always that easy. They sometimes really try to hide key dimensions
2 Likes
Easier than redoing my prototype and sending off to the fab again. 
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.