I used Connector > Molex_Mini_Fit_Jr_5566_20A_2x10_P4.20mm_Vertical and when my board arrived I found the pitch (between rows) was 5.50 mm not the P4.20mm stated. I have checked the footprints in KiCad and it seems all the different footprints of this style are the same wrong value, ie all footprints from 2x1 up to 2x12 pins and both Vertical and Horizontal layout.
There is an old post from Apr 2017 that mentions this: https://forum.kicad.info/t/potential-incorrect-footprints-for-mini-fit-jr/6006
so its a very old problem, and not just a single footprint.
Edit: To be clear, I have since downloaded the footprint direct from the Molex website, and that downloaded footprint also has pitch 5.50mm, but the component I bought has the 2 rows at 4.20 pitch, as defined in the name.
Searching online, this connector is used for PC power supplies, and the pitch is described as 4.20mm, eg https://en.wikipedia.org/wiki/ATX
" The connector pin pitch is 4.20 mm…(about one sixth of an inch)."
From old forum thread you pasted above seems like some knock-offs of the original Molex connectors have 4.2mm row spacing, so probably yours is not original Molex.
This is a very confusing part where the plug/socket pin to pin pitch is 4.20 x 4.20 mm, but the PCB pitch is 5.50 x 4.20 mm.
Normally in connectors we are talking about the plug/socket pitch
Edit: Paulvdh: I changed all the "4.40 mm sizes to 4.20 mm. This is both shown in the footprint loaded into KiCad (Molex_Mini-Fit_Jr_5566-20A2_2x10_P4.20mm_Vertical) and on the screenshots shown here.
What I am saying is that the socket I bought to go on my board does not fit the 5.50 mm between rows, and my PC power supply fits into the socket I bought. So my 2 items are 4.20 pitch in both directions.
It would be strange if someone was trying to sell knock-off items that are wrong.
This is a diagram of power connectors:
On my computer screen, the pins are equally spaced pin pitch and row pitch, and the pitch is nearer 4mm than 5mm.
Read the comment from the old forum thread you sent a link earlier.
Molex is 4.5 / 5.2mm, while cheap Aliexpress knockoffs are 4.4 / 4.5mm.
So I’ll say that again - looks like your is not original Molex. So Molex footprint may be (and in this case it not) correct for your connector.
the receptacle holes are indeed 4.2 mm apart in both axes. But the pad centres are 5.5 mm apart, probably because the pins are “turned outwards”. Have you fitted pins into the receptacle yet, or are they prefitted?
Sorry for the delayed response. Somewhere in my design process there must be an error, but I can’t find out where.
I bought a power supply first (Seasonic SS-250SFD MicroATX).
Seasonic (https://seasonic.com/about-us/) claim to have been supplying this market for 45 years and I think they are reputable.
I then bought a connector for the board, admittedly on eBay, but it fits on to the PSU cable harness. It already has the pins in it.
I then designed the board, and expected the connector to fit.
There is no obvious kink in the pins of my connector, but the diagram of the Molex MiniFit also shows straight pins. As previously stated, I measured the row spacing to be 4.20 mm on the connector on the end of the power supply cable.
I am lost. It seems inconceivable that the specification on the web of all those Molex connectors is wrong, and similarly for the KiCad footprints.
Thankfully this was a design test board - I just don’t know how to proceed for mass production.
Don’t buy at eBay for mass production, but from a reliable source that actually sells Molex.
I had a similar situation with a local suppliert that sold us “compatible” 2 pole Wago- connectors. They were wider and no longer fitted through a slot in the cases already machined for … wait for it … Wago. That’s how you save not just pennies in production.
I tried to read this thread again more carefully, and also the old thread you referred to. I still not sure if I (we) have not understood you correctly, or if you haven’t understood the issue and the answers. The older thread boils down to the same conclusion than the answers in this thread: the “official” pin pitch between the two rows is 4.2 in the connector/connector (jack/plug or female/male or board connector/wire connector) interface, but 5.5 in the interface between this connector and the PCB. This is correct if you have a legitimate connector.
Or not. “Strange” is a subjective description. It’s possible that they are just cheaper to manufacture. And who has ever claimed they would be identical for the PCB contact? To be compatible for their normal purpose they only have to be compatible with the other connector.
I understand you have been mislead by the footprint name in the Connector library, but please remember you have to always check every footprint you use before trusting it.
What specification? To me it looks like only the footprint name looks misleading. But note the Molex page for the corresponding item, https://www.molex.com/en-us/products/part-detail/39281203 (which is in production and has a link to the up-to-date datasheet) and read the description. It says 4.20 mm pitch. Yet the datasheet shows the information just like you described in your OP: 5.5 mm pitch for pins which go into the through holes in the PCB (center to center); 4.2 mm for the connection pins for mating the wire connector. Everything is correct in the original Molex connector, the datasheet and in the KiCad libary, the only problem with regard to them is that you seem to have interpreted the footprint name to mean 4.2 footprint pitch.
So, what do you say? Has Molex described it wrong? How should the KiCad library name it? Would the footprint name be correct if it would be named contrary to what the manufacturer says?
Finally,
Isn’t it obvious this far? You have bought a replacement part which isn’t identical to the original. Everything else matches and is correct, although I admit that the footprint name may cause misunderstanding.
