I've recently added the ADC Microcontrollers ('C265 and 'C134) to my KiCad symbols library.

However, I cannot find mechanical drawings of the QFP parts to determine which pin pitch they're using. Does anyone happen to have these parts or otherwise know the correct pin pitch for these parts?

(in actual fact, as far as I can tell the 'C51 ACIA is the only WDC part that has mechanical drawings in its datasheet, which is ironic given its probably the least used of their parts, but for all the other parts so far I've either been able to infer pitch from other sources or I've actually bought the part - but not in these cases)

_________________
Want to design a PCB for your project? I strongly recommend KiCad. Its free, its multiplatform, and its easy to learn!
Also, I maintain KiCad libraries of Retro Computing and Arduino components you might find useful.

You may look at https://www.microchip.com/en-us/support/package-drawings and select PQFP packages.

Whilst I can't answer your question I can a little more confusion.

The W65C816S6TQG-14 appears to use what Microchip call the 44 Lead Atmel Legacy- K package. Not the 44 Lead KW package.i.e. its width is 13.2mm not 13.9mm. The pitch is 0.8mm for W65C816S 44 lead PQFP regardless so if you're only interested in the pitch then each of 100 lead PQFP packages are all 0.65mm and the specific package doesn't matter.

However there does seem to be a bit of variance in the overall lengths (23.2mm vs 23.9mm) of the PQFP 100 lead packages so probably best to design your footprint for the larger version.

(Again for the W65C816S) I've used a footprint of 14.5mmthat I could comfortably solder. The adapter board (pictured) only had a width of 13.0mm and was complete pain to work with.

So, the W65C51N ACIA I know has a pitch of 0.8mm because it says so in the datasheet, it also explicitly says it is an LQFP package (not PQFP).

For the QFP-44 package used by most of the other WDC devices (W65C02, W65C22, W65C816), there is only one pitch of 0.8mm which does make life easier. By similarity to the ACIA I used the LQFP footprint, but I could change it to MQFP to make hand soldering a little easier. I actually have some of these parts - somewhere - so I'll measure them later today.

The leaves the W65C134 (80 pins) and W65C265 (100 pins). The QFP-80 packages comes in 0.4mm, 0.5mm, 0.65mm and 0.8mm pitch varieties. QFP-100 comes in 0.4mm, 0.5mm and 0.65mm pitch varieties. Since the datasheets are completely mute on the issue, and I don't own either part, I have no idea which pitch they should be. This is where my problem lies. =

I would be happy to buy one of each to measure (indeed, I'm planning on using the '134 in a project which is what has precipitated the update to the symbol library), however the QFP versions of these parts seem to be very hard to get in the UK, so I have resigned myself to using the PLCC version for my project.

_________________
Want to design a PCB for your project? I strongly recommend KiCad. Its free, its multiplatform, and its easy to learn!
Also, I maintain KiCad libraries of Retro Computing and Arduino components you might find useful.

Yeah, it's more than just a bit frustrating. But I had a bad idea!

The size of the W65C265SXB and W65C134SXB single board computers is known (both PCBs being 2.5 inches by 3.25 inches)You could measure a component like a pin header or use the board size to measure the pitch off of the '265 or '134.

I'm not brave enough to commit to a footprint based on a blurry photo but hopefully it'll give an indication of the pitch (which seems to be 0.65mm based on 30 leads on the 20mm long side).

That is a really good idea, to look at the pictures! Thank you!

That has allowed me to narrow it down to the correct pitches, because from those pictures I can see both chips are rectangles not squares, and in each case only one pitch option is for a rectangular package.

Therefore, I can say with some certainty that the QFP-100 package measures 14x20mm and is therefore pitch 0.65mm, whilst the QFP-80 package also measures 14x20mm and is pitch 0.8mm.

_________________
Want to design a PCB for your project? I strongly recommend KiCad. Its free, its multiplatform, and its easy to learn!
Also, I maintain KiCad libraries of Retro Computing and Arduino components you might find useful.