This is something that’s usually equally miserable - but different - across different systems.
I need a double-sided card edge connector (2x36, which is itself a little unusual). I don’t
want a single schematic symbol, rather 72 separate connector pins I can scatter about
the drawing. What I don’t know is which symbol attribute is used to correspond with the
appropriate pin on the layout symbol and where the correlation is defined.
You have to create a single symbol male, female (or diverse) depending from your needs. The symbol entry for your edge connector then uses 72 units with one pin each. You may scatter the placement of the single pins anywhere in the schematic. You may mirror some pins to draw from left to right following the signals from input to output. You are allowed to stack them in groups of columns only having the top pin with visible reference designator. Switch the reference Designator of pins below to invisible after you made sure they are assigned correct You are allowed to draw a group of unused pins in the corner of your sheet to maintain overview of unassigned pins.
Open the symbol editor with a 4001 IC and examine how the Units are made and then you understand how Kicad symbols work
Do it another way. Put a connector symbol on your schematic. Attach a unique label to each pin. Use the same label elsewhere in your schematic to make a connection that that connector pin.
Appropriate in some cases, but not this one.
[quote=“janvi, post:2, topic:39236, full:true”]
You have to create a single symbol male, female (or diverse) depending from your needs. The symbol entry for your edge connector then uses 72 units with one pin each. You may scatter the placement of the single pins anywhere in the schematic. You may mirror some pins to draw from left to right following the signals from input to output. You are allowed to stack them in groups of columns only having the top pin with visible reference designator. Switch the reference Designator of pins below to invisible after you made sure they are assigned correct You are allowed to draw a group of unused pins in the corner of your sheet to maintain overview of unassigned pins.[/quote]
Yeah, that’s standard practice, but the implementation details are what differ. I’ve
already laid down my 72 discrete pins, but didn’t know where the info correlating
the symbol with the layout footprint is kept. Thanks for the 4001/Units pointer - that tells
me the mapping is kept with the schematic symbol and not somewhere more obscure.
Btw, in the system I’m accustomed to, that correlation is contained in a “map” file
describing the schematic symbol, how many of them, and how their pins connect to
the layout symbol’s pins. You can use a graphic editor to join them up, but the map
file is ASCII, so (especially in the case of high pin counts) it’s a lot easier and faster
to just bust it open with vi and edit it directly.
Symbol pins are associated with footprint pads by the pin names which have to match up with the pad names. Usually the names are numbers because a lot of footprints use numbers like DIP packages. If you are making both yourself you’re free to label them how you like.
Thanks - that helps a lot. Old card edge connectors can sorta be a pain because often
one side is numbered and the other lettered - and worse, some letters are omitted (to
avoid confusion they typically don’t use I, O, Q, etc.) and once they’re past Z they go to
AA, etc. I guess you can look at it as being a little like DIN 41612 (i.e. alphanumeric), but
with less consistency and more annoyance. And to cap it off, the company whose gear
I’m reverse-engineering reversed the connector for no good reason whatsoever, so the
letters are on top, numbers on the bottom, and all increment right-to-left. Whoopie!
Anyway, being able to designate both a symbol node and footprint pad “AE” will make
things a lot easier.
Perhaps this will help clarify…
Say you have a Device ‘A’ with 100 pins and want some of the Pins connected to Device ‘B’ and some connected to Device ‘C’…etc and, they can be on separate schematics…
Say, for graphic clarity, you want the devices at different locations on the Schematics (naturally, the actual Device ‘A’ on the PCB will need Traces to Device ‘B’ and Device ‘C’…etc on the PCB.
Example below shows the Device ‘A’ (dumb_2_36 but, could have 100 Pins…) and three other Devices. Nuturally, you can Label as desired (I practiced Spanish counting)
Annotating (click the button) will associate the Devices according to the Labels shown. Updating the PCB from Schematic will load associated Footprints and will connect them with Rat-Lines per Label association. Then, you simply route your traces or use an Autorouter. The Schematic symbol’s can have Footprint with 3D-Models associated with them.
There are Net-Labels, Global-Labels and Hierarchical-Labels to use as needed.
And, the PCB’s Pads and Traces will show the associated Net’s (if your graphic pref’s are set to show them). last image
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
