Incorrect footprint dimensions?

[ratio]

Working on a (learning) project in KiCAD, I decided to make a footprint for a bridge rectifier. I couldn't easily find a pre-made footprint, so I made one using the dimensions from the data sheet (http://www.mouser.com/ds/2/258/GBJL35005-GBJL3510(GBJL)-272221.pdf). Set the snap grid, dropped the pins, but when I drew the outline, using the snap grid and math, I came up with the attached. Is the data sheet ...erroneous?  I used the metric dimensions, but the imperial numbers seem to be within conversion tolerances.
On a side note, does the shape of the bridge have an official name? I'm looking for a heatsink for it, but I'm too green to just know of one offhand.

[mikerj]

Probably just tolerance stack up.  Which measurements did you use for the package and pin spacing: minimum, maximum or half way between?

[phil from seattle]

This is a never ending struggle.  The footprints you find on the internet are often wrong.  I'd trust the datasheet over anything you find. 

But datasheets have errors too so best to have an actual part and a pair of calipers.  I'd also print the board on paper at 1-1 and see if your pads line up with the actual device.

I'd drawn a footprint from a datasheet and had a board made without having the actual part in-hand. Sadly, the datasheet had the part numbers for the two variants of the part backwards. So,I was thinking "I'm soooo smart to speed things up".  Until I discovered that I had to fix and reorder the PCB. Definitely a learning moment.

[saike]

I just drew this out of interest and got the same result as you. Add the F, N, O, O dimensions and you get the A dimension.
Get the component and measure it.

Edit: The A dimension within a fraction of a mm.

[ratio]

I used the center of the mm dimensions. I figured the tolerances aren't additive. My guess is that the outline is wrong, I was just wondering how common something like this is.
Another question that I forgot to ask: I drew the holes following: https://www.pcb-3d.com/knowledge-base/pth-dimensions/, with what it claims are IPC-2222 level A tolerances. Does the copper look scant?

[floobydust]

Another manufacturer has 2.5mm vs 2mm "F", and 30mm width vs 27.5mm "A"
GBJ35x.pdf

3D .step models:
https://grabcad.com/library?page=1&time=all_time&sort=recent&query=rectifier
http://www.3dcontentcentral.com/Search.aspx?arg=bridge%20rectifier%20kbj

[mc172]

It models up OK for me using the min. dimensions. It looks like you might have taken F from the edge of the pin rather than the centre in your footprint but the dimensions on the datasheet are not great.

If you model it using nominal values the furthest right pin ends up outside the package. I think it's due to someone not understanding the implications of tolerancing. They probably asked the marketing department to "make up some tolerances comparable to what our competitors are doing".

I used the min values for each dimension and it all looks OK in SolidWorks. You can probably safely assume that the pin pitches are correct, and centre the rest of package around the pins at the maximum dimension.

Image attached is minimum dimensions working, but nominal and maximums do not work.

[ratio]

Thanks. I ended up drawling it with the 2.5/30 mm dimensions mentioned by floobydust, with that hint I found a few more datasheets for an (I hope) analogous part, they all agreed with the 30 mm.
It would seem that GBJ is the form factor. I had less luck finding a heat sink from a reputable source, although sleezBay does have something that looks like it'll work.