I recently installed 5.1.2 on my system, and realized that the SO8 (SOIC-8_3.9x4.9mm_P1.27mm) footprint’s pads goes waay under the footprint body. Is this intentional?
It is script generated with IPC rules and settings:
SOIC-8-1EP_3.9x4.9mm_P1.27mm:
size_source: 'https://www.analog.com/media/en/technical-documentation/data-sheets/AD8210.pdf#page=15'
body_size_x:
minimum: 3.8
maximum: 4.0
body_size_y:
minimum: 4.8
maximum: 5.0
body_height:
minimum: 1.35
maximum: 1.75
overall_size_x:
minimum: 5.8
maximum: 6.2
lead_len:
minimum: 0.4
maximum: 1.27
lead_width:
minimum: 0.31
maximum: 0.51
pitch: 1.27
num_pins_x: 0
num_pins_y: 4
The problem here is the very high tolerance for lead length which means that it must be expected that the leads are bent inwards in extreme cases.
I have never seen that or even close to vertical. Are all the tolerances truly independent?
They are not completely independent which is why IPC does not simply add tolerances to arrive at the resulting expected contact area.
The formulas are of the form: Smin(RMS) = Smax - √(Sum(tolerances²))
In this case having 1.27mm contacting lead length will get the contact area under the body even if the outside to outside dimension is at its maximum.
If i enter the same dimensions into eagles generator i get the same footprint out. Meaning my generator can not be totally wrong. (It is more likely that the SOIC specs simply are extremely cautious.)
I don’t think it is possible to bend the pin under the body. Were there any problem with the old footprint?
It is not necessarily to allow for pins bend under the body but to have enough space for proper solder fillets no matter how the leads look like.
And we are generally replacing all manual made footprints with scripted ones but that simply takes time.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.