Eagle interfacing connectors
Part of Eagle Training.
Table of Contents:
Making connectors that interface between multiple boards is a critical thing to get right whenever there is a design with multiple boards. Any number of things can go wrong: the spacing between connectors could be different and the boards can plug in, one board could face backwards, the pinout could be mirrored, signals could be left unrouted, some boards might not fit, and the list goes on. The goal of a good Eagle connector between two boards is to prevent all of this.
Aside: Making a good interfacing connector is restrictive, and that's good. But early in the design cycle when things are changing more, that is a disadvantage. Wait until layout is mostly complete before making an interfacing connector between two boards. Until then, just use some block of which connector you eventually plan to use.
In this tutorial, I will use the example of the X12 QuadESC to Backplane connector. IMO, this was lacking in several aspect, so there's lot of learning examples, and I can point out what not to do and what to do.
First: There are the signals. Group them logically/sensibly like you would for an IC. Something like power on top, ground on bottom, in on left, and out on right. Or I/O on both sides depending on the board. The original design has two blocks that look like this. Not only are the pins using the default "P$..." name, which is extra long and hard to read on a schematic, it gives me no indication of what signal must connect where. Let's change that to have the signals we need: 12V, GND, 3.3V, CAN_H/L, and programming select. If you're been using the pinswap feature, I recommend you disable it by setting all pinswaps to 0.
Key things for the symbol:
- One symbol for everything (even if multiple connectors)
- One pin per signal (no having GND multiple times)
- Place pins in a reasonable layout
- No pinswap!
Original Symbol (left) and Improved Symbol (right)
Ahhh. That's better.
Next up is the footprint. Boards that stack on top of each other are much each because the pinout doesn't need to mirror. Boards that are coplanar and connect via right angle connectors might need to flip or mirror the pinout. You should already have the footprint whichever connector you are using in the library. Copy the footprints around and position them as they should be on the board. You may want to rename all the pins to the signals they connect to (12V@1, 12V@2, etc...) or you can just name them 1, 2, 3, etc. I'll do the former. After this is done, you should draw an outline of the smaller board on the tDocu (51) or bDocu (52) layers. This does two things. First, it makes it clear if the connectors are positioned properly on the smaller board. Second, it makes sure that the other board doesn't put it somewhere where it collides with other things (walls, boards, etc). This actually happened on the first order of this backplane. It's also good to put boxes on t/bKeepout layers (39 & 40) to signify which side of the board the connector will be on.
Original Footprint (left) and Updated Footprint (right)
When you are satisfied with the footprint, go to the table of contents and duplicate the footprint. Now change things from the top layer (tDocu, tKeepout, etc) to the bottom layer (bDocu, bKeepout, etc) or vice versa so that the board it connects to has it on the right layers.
Key Steps for the footprint:
- Place box on 39-tKeepout and 40-bKeepout to indicate side of board (and prevent other parts from intesecting)
- Name Pads/SMD numericallys (1, 2, 3, ...) or by signal (GND, 12V, ...)
- Think about how the connected is / will be keyed and do that effectively.
- Add board outline on 51-tDocu/52-bDocu
- Duplicate and switch everything to top/bottom once the footprint for one is fully complete.
Now onto the last step. Make a new device and add the symbol you make in the first part. You can either make two devices, or make one device and have variants for the two boards (ESC and BKP in this case); I will be making variants. Add the footprint you made with the outline and connect the pins. Multiple pins from a footprint can be connected to one pin in a schematic. If you named the pins after their expected signal, this part should be easy. If not, you just need to give it some thought and do it right (and consistently for both).
Orignal Device (left) and Updated Device (right)
If you're adding step files for Mechanical CAD models, now is a great time to add them.
You're all set! Just add it to Eagle, connect the signals, and rest with piece of mind that you board will connect properly.
Original Board (left) and Board with updated part showing the issue of boards overlapping (right)