44 pin plcc to pga adapter footprint

[Steve Crompton]

Hi there,

I need to create a pcb library part for a 44-pin PLCC IC Socket

I have found the following diagram and was wondering if people can cast an eye over it and confirm this is the correct pinout and dimensions

I don't have a socket to check - I have them on order

Thank very much

[Mark T]

It matches the pinout of epm7032s44, plcc 44 socket in eagle, assuming top view, though I have never used that footprint yet.

[Sergey Kiselev]

Yes, the pinout looks good to me. It matches the pinout of PLCC44 TH socket, and my own PLCC44 footprint, which I did use in my projects and I know that it works.

[Rob Gowin]

On Saturday, December 19, 2020 at 6:28:39 PM UTC Steve Crompton wrote:

Hi there,

I need to create a pcb library part for a 44-pin PLCC IC Socket

I have found the following diagram and was wondering if people can cast an eye over it and confirm this is the correct pinout and dimensions

I don't have a socket to check - I have them on order

Hi Steve,

I agree with Mark that your pinout looks good. Have you considered using the convention of having pin 1 be a square pad? I've found that helpful.

I've used the footprint available in KiCad successfully. Compared to that, your drill hole diameter of 0.8mm/31.5mil matches KiCad. Your solder pad diameter of 1.1mm is smaller than KiCad, which uses a diameter of 56 mil/1.42mm.

Alternatively, this data sheet [1] uses a drill hole diameter of 0.9mm/35mil, solder pad diameter of 1.5875mm/62.5mil. It suggests an overall X dimention of 23.2mm/913mil.

Rob

[1] https://www.mouser.com/datasheet/2/273/144-259668.pdf

[Bill Shen]

The pad numbering is correct.  The 1.1 mm diameter pad is really quite small, especially in relation to the 0.8mm drill.  In my PLCC44 library I used 12.7 mm pad and 0.7mm drill.  0.7mm drill is a bit tight, so 0.8mm is better, but then the pad diameter need to be correspondingly bigger, like 14mm.  As long as pad is smaller than 15mm, you can route 2 traces through.

Yes to square pad for pin 1.  You'll thank yourself when debugging.  The socket is nominally 23mm x 23mm, so the component outline is a tad too small.  Just don't place components right up to the PLCC44 outline.
  Bill

[Tom Storey]

Hi Steve,

The pinout seems correct according to some recent work that I have done.

But which PCB CAD are you using? Seems crazy that it wouldn't already have such a socket that you could copy out of an existing library?

e.g. in EAGLE you will find a few sizes in the "plcc-socket" library. I would be surprised if something like KiCad didn't have something similar. I would tend to copy a footprint from another library rather than designing one from scratch if I can, but I would take my own measurements against the devices datasheet afterwards to make sure it is physically correct.

Unless you just want the experience of building your own parts, in which case ignore me. :-)

--
You received this message because you are subscribed to the Google Groups "retro-comp" group.
To unsubscribe from this group and stop receiving emails from it, send an email to retro-comp+...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/retro-comp/7fb67126-1f70-4edb-8641-d71531ca90fen%40googlegroups.com.

[Steve Crompton]

Hi Tom

I use diptrace, there are larger PGA parts in the library but what I was most interested in was the pin numbering - I could not work out where pin one was on a 44 pin package

I took one of the larger packages and scaled it down renumbering the pins - all done now, just hope it works out correct

Steve

[Steve Crompton]

Thanks to everyone that contributed to this topic - all comments taken on board

Job is now done

Hopefully part will work out as expected when it comes to the PCB :-)