AMP - TE CONNECTIVITY 1-828584-6 Wire-To-Board Connector, Right Angle, 2.54 mm, 16 Contacts, Header, Through Hole, 2 Rows
or something equivalent to it. I don’t mind adapting one with fewer/more pins, I just don’t feel confident in making such a part from scratch at present.
If I need to make my own, am I right thinking that I would be advised to start from a 2x8 pin header footprint? I would appreciate advice on specifically which kicad library part.
Well, to start with, you don’t make it from “scratch”. You use the tools in KiCAD Footprint Editor to make it from loose digital bytes rattling around inside your personal confuser. Ecologically responsible people will use recycled digital bytes. “Scratch” is what my wife uses to make my lunches.
Find the library for “Pin Headers”. On my installations, it’s at {KiCad Install Folder}\share\kicad\modules\Pin_Headers.pretty
Does the footprint “Pin_Header_Angled_2x08_Pitch2.54mm” give you a good start on what you need? This footprint doesn’t seem to apply to a shrouded connector, so you’ll have to increase the courtyard area to accommodate the shroud, the latching fingers, and an allowance for the mating connector to slide in and out. You’ll probably have to add an unplated mechanical mounting hole or two.
Be careful when you identify “Pin 1”. Not everybody who makes this style of connector agrees on how pin numbers are assigned.
Dale, thanks for that spot - I hadn’t noticed. I wish electronics shops would defatult to ‘avtive’ stock!
Re the pinheader, I am worried that I get something wrong with the mechanical design which I only discover after manufacture! I’ll give that header a go.
From my perspective you could likely use the aforementioned 2x5 or 2x8 or 2x?? header with the correct pitch “as-is” (from the photo I only count 10 contacts… you state 16, which is it??)
The only reason to change the “courtyard” or footprint is so the silkscreen matches, which is a good idea. But the main thing, as you likely already know is that the pin pitch and hole size matches your actual part.
It is super simple to grab a caliper and measure and expand the silkscreen to match your part. Add a couple of holes for mechanical mounting, if needed and you should be good to go.
As dchisholm mentioned BE SURE to check the pin numbering of the footprint and make sure it matches the schematic symbol. (that just bit me on a board I had made) it’s easy to correct by just right clicking on the pin numbers and change them to match your schematic symbol. If you don’t do this step the board will be wrong. (and you should do this check for EVERY part on your board that is sensitive to pin numbering (ie… not resistors) otherwise the rats-nest and subsequent pcb traces will terminate to the wrong pins even if the label or silkscreen says you are connecting to the correct pin)
Finally, while you are editing the footprint in the editor, be sure to change your active library to your personal lib (you do have some sort of personal lib of tested components don’t you?? if not start now) then save the edited component with a new appropriate name and it will now be available in the future.
And pat yourself on the back you have just made your own custom part
Hi, if you dare to try FreeCAD, you can get easily the footprint checking through the mechanical 3D part TE C-5499345-3 3D model STEP http://www.te.com/usa-en/product-5499141-3.html#pdp-docs-features
after having the model you can import the footprint in FreeCAD using kicad StepUp and align the Part to its footprint, then you can project the 3D model to obtain the 2D path of the model and export it to dxf; after that importing the dxf into kicad footprint editor you can add the model path as silkscreen and add the STEP/WRL 3d model to footprint…
Thanks, guys, for your assistance here. The connector I was thinking about is indeed 2x8 - 16 pins - it’s just that the pic was for a different size. Not sure I’ll play with FreeCAD yet – there are too many other projects on the go – but good pointer anyway.
I was thinking that the latch arms would hang over the board edge – don’t want to waste the board space – but worth remembering that stuff anyway.
I had a look at the 3d view of my current effort last night and it was without a PCB… components all floating in space. I guess I’ve left something out of my design, but what?
Finally, my board will be a Beaglebone cape, so I have used a schematic that includes ‘pins’ for the expansion connectors and built a ‘footprint’ for them, with marks for the board edge and mounting holes to align to. This footprint uses footprint pads to make the holes with the right names and act as the physical side of the schema pins.
I do need an actual pin header too, though, which of course has its own pads, and so of course the two sets of pads conflict. The only thing I can think of doing is make a new footprint for the connector which doesn’t actually have any pads. It seems icky, but is that the best option?
I have not played with the 3d viewer much. Have you defined the Edge Cuts outline? And if you have make sure there is no break in the edge cut outline.
As far as the pin headers that feed straight through… If I understand correctly you just want the pin/socket headers to be soldered into the cape and not have any connection?? If so then you should be able to add the appropriate pin count header or connector to the schematic and then place a not-connected-flag (its the x symbol on the right side tool bar) for each of the pins that you just want to pass through. This way you can assign whatever PCB footprint to the header and have a standard hole and solder point.
The no-connect will also allow the DRC check to go without error for those unconnected pins.
If the module has only ONE connector (=1 physical part that needs ordering) you can do this:
If there is more than one connector (gumstix for example has TWO) the footprint for the hat/cape/motherboard/etc. will only contain markers and center marks for the connector footprints, otherwise you can’t align them.
The schematic would need custom schematic symbols then (which carry the correct pin names) and have a link to the connector footprints.
The BB is designed with two 40-pin connectors, in a similar way to the RPi 2 & 3; the actual connector to be used, though, depends on the cape: sometimes you will use fewer pins, or even omit one side altogether.
What I have at present is a schematic symbol that splits out the various pins across 4 units (one for each connector row), obviously each unit is unique.
I have also made a footprint, together with a board edge line (I put it on the User.Cmnts layer) and “pads” to represent the board mounting holes. [Why isn’t there a dedicated ‘drill’ thing that has no ‘pad’ semantics?]
So this is 1/4 of my schematic: the others are similar:
