Yes, I will use backups 
Still after a week not a single crash. 4.07 crashed about every time I used it.
v5 still lacks a lot of 3D models: my board is almost empty in v5. Only capacitors and resistors. No LED’s, no SOT housings etc.
The only weird thing I discovered are SOT-23-5 and similar chips are that I was used to having pin numer 1-5 for these symbols, but now the footprint uses pins 1,2,3,4 and 6! So I had to change my symbols!!
I wonder if that is intentional or just a mistake !
Sounds like a ‘problem’ with the footprint generator.
It leaves out pin #5 but doesn’t remove one from the count for physical pin 6, so it is being applied #6 instead of #5.
Might pay to visit the library on github and post a bugreport there, to see what the people in charge think of it?!
I am not sure what library you use but the SOT-23-5 footprint in the official lib looks like this:
I see pin numbers 1-5.
Moved to a new topic
I checked my board, and here is the footprint that I used.
Package skipping pin 5:
I needed the 0.95mm Pitch, Thin SOP…
Other footprints show the same things in this package Package_SO.
So maybe I’m using the wrong footprints for my symbols in this case??
Package skipping pin 7:
so your wrong fp is not sot23-5 but TSOP-5
kicad fp TSOP-5
and an other wrong is the second one you posted
kicad fp SOIC-8-N7
You should rise an issue at GH repo
so your wrong fp is not sot23-5 but TSOP-5
Yes, I was mistaken, mixed up SOT and TSOP
You should rise an issue at GH repo
Will do that!
SOIC-8-N7 is not wrong. The N7 tells you that the missing pin is the one with number 7.
From the datasheet:
However the TSOP-5 should indeed be numbered 1…5 at least if we go with the numbering as mentioned in the vishay datasheet that is used in the description.
Pull request with the fix for that: https://github.com/KiCad/kicad-footprints/pull/509
Onsemi use 1-5
Anyone with an example of the 7 pin SOIC N7 part?
NCP1207B in the official lib
Odd, the Onsemi datasheet shows a regular SOIC 8 pin with pin 7 nc and a comment about clearance distance. It would be very unusual to have a non standard lead frame
You have to be very carefull with these small SMD footprints.
Most often pins are numberd counter clockwise, but sometimes they are numbered clockwise.
It’s a lack of standardisation. Hopefullly this has improved over the years, but it is one of the things that unfortunately have to be checked carefully to be sure.
Over the last few years the packages of small SMD resistors and capacitors is becoming ambiguous.
A “0603” can be “metric” or “imperial”, with a big impact on size.
Sometimes there are also (very) small differences in pitch between seemingly similar packages.
Stuff like this is one of the many resons that you should never rely on standard libraries for a final PCB design. Always make a separate library for a project, or maintain your own set of verified libraries for schematic symbols and footprints.
This onsemi datasheet has both the 7 and 8 pin variant. http://www.onsemi.com/pub/Collateral/NCP1207B.PDF
(See right half of page one)
This is why the 0603 (imperial) resistor is called R_0603_1608Metric in the official lib
Thanks, I was looking at an older version without the 7 pin variation.
Unusual in small signal parts, but rather more common in mains switchers, which I believe are the main parts using such a isolated pin 8, (no pin 7), as they often have 700V pin ratings
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.
