Re: gEDA-user: QLP packages?

[Dan McMahill <dan@xxxxxxxxxxxx>]

Matthias Wenzel wrote:
> John Luciani wrote:
>
> > QLP (quad leadless package) may be similiar enough to the QFN (quad
> > flat no-leads) footprints that I have created.
>
>
> Well, they aren't similar enough. Just have a look on
> QLP20 page 64 in http://www.chipcon.com/files/CC1100_Data_Sheet_1_0.pdf
> QFN20 page 54 in http://www.chipcon.com/files/CC1070_Datasheet_rev_1_2.pdf
>
> > I have a couple of QFN packages (including a 20 pin device) at
> >
> >   http://www.luciani.org/geda/pcb/pcb-footprint-list.html#QFN
>
>
> BTW: why don't you use /usr/share/pcb/m4/qfn.inc macros?
>
> Matthias

Actually, it looks like QFN and QLP are quite similar and probably close 
enough.  You're comparing the QLP to the wrong 20 pin QFN (welcome to 
the world of modern packaging).  There are 4x4mm and also 5x5mm 20 pin 
QFN packages.  One has a 0.5 mm pitch and the other has a 0.65mm pitch.

check out the ~geda library, QFN20_4_EP and QFN20_5_EP for the 4x4 mm 20 
pin and 5x5 mm 20 pin QFN packages.

In IPC-7351 these would be QFN50P400X400-21N and QFN65P500X500-21N for 
the nominal footprints.  The "21" is 20 pins + the exposed paddle (the 
big pad underneath).  The 50P vs 65P is 0.5 mm vs 0.65 mm pitch. 
400X400 is 4.00x4.00mm and 500X500 is 5.00x5.00mm, and the "N" is for 
nominal.  Looking in the land pattern viewer I see

QFN50P400X400-21V1N  -  1.0 mm height
QFN50P400X400-21V5N  -  1.0 mm height
QFN50P400X400-21W1N  -  0.8 mm height
QFN50P400X400-21W5N  -  0.8 mm height

QFN65P500X500-21VN   -  1.0 mm height
QFN65P500X500-21V2N  -  1.0 mm height
QFN65P500X500-21WN   -  0.8 mm height
QFN65P500X500-21W2N  -  0.8 mm height

I didn't compare the IPC land patterns to the QFN packages in ~geda but 
my guess is that they are ok.  I've ordered a board with the QFN68_10_EP 
footprint from ~geda and it seemed ok.


-Dan