Hello !
Is there a reasonable scenario where a footprint (or parts thereof) are drawn on the bottom side of the board ? By default everyone sets up a footprint on the top side. I’m not aware of such a scenario. Maybe others out there ?
Mario
There can be instances of features unique to two sides of the board. For example, a processor socket where there need to be features on the bottom side of the board to remind layout not to put components where a heatsink clip would go.
Personally, the only time I’ve done this is when designing footprints to use as an Arduino shield. Features to indicate clearance areas on the underside for expected tall components of an Arduino, and features on the top like pin signal labels. I would imagine something similar for R-Pi Hats, but I haven’t designed any of those.
But if I’m designing a footprint for something that I know that I plan on using on the underside, I’ll still design it on the top side and then flip it during layout. Makes it easier to design without having to mentally flip dimensions and text.
I ttried do something like this and it did not work. It wasn’t important at the time, but i realise now that it might be a bug.
What i wanted to do was create a fiducial that would be placed on the front of the board, but would also have the same features on the back.
So i created thr fiducial footprint with an smd copper pad on the front and a pad with the same dimensions on the back (placed at the same coordinates).
I did a quick test and placed the footprint on the board and it showed the two smd pads on the cortrct layers.
However, The gerber outputs would only show the front pad, never the back.
I decided then that i would just use a fiducial designed for the front layer and flip it.
Of course with THT pads and mirrored layers it’s not a problem, but with SMD pads it could be.
That’s the way to do it.
Take a pcb with components on both sides: if you flip physically the board you’ll see that components are always on the top side (from the point of view of the component).
A footprint designed on the bottom layer, viewed from the top layer in the layout as every CAD program does, will be rotated on the X or Y axis, definitely useless.
Some microwave filter structures would have associated pads but different pads top and bottom. I don’t think KiCad can do this
Some microwave filter structures would have associated pads but different pads top and bottom. I
can you give an example ? A link to such a component or a photo would do. Thanks.
There can be instances of features unique to two sides of the board. For example, a processor socket where there need to be features on the bottom side of the board to remind layout not to put components where a heatsink clip would go.
Good idea. this approach would affect the person who is doing the layout. The assembly folks won’t notice such a feature as it is not part of the bottom silk screen, right ?
Do “reverse mount” components such as LED’s and phototransistors qualify ? These are soldered to one surface of a board, and poke-through a hole to the opposite side. Reverse-Mount LED
Dale
If with parts thereof you include smd pads then there are a lot of examples in the official lib.
See for example this _ThermalVias footprint.
If you limit it to fab and silk drawings, then there are for example the phoenix contact connectors in the lib with mounting screws.
(The connector is on the top side, the screw head is on the bottom.) This needs to be communicated with the layout guy as there should not be traces between the pcb and the screw head. To achieve this we include a circle on B.Fab to communicate this with the layout guy and on B.SilkS to also show someone manually assembling this what size the head should have.
Other examples are connectors where there is no way of marking pin 1 on the bottom side (we normally use a rectangular pin only for pin 1 of a THT component. Some footprints require all pads to be rectangular. In such cases we add a silk marking for pin 1 on the bottom to make debugging easier.)
Example: Molex_MiniFit-SR-43915-xx06_2x03x10.00mm_Straight
And there are also things like edge connectors.
That all depends on how you design the footprint. Personally, I would probably include an outline of the expected heatsink clip on the underside so it would show on the finished board. Some people don’t like silkscreens and only use fabrication layers to communicate to assemblers so they wouldn’t put an outline on the silkscreen.
1 Like
very good reasons ! Thanks for clarifcation 
Parts that mount on an edge of the board will often have pads on both sides. Take, for example, this USB C Plug connector.
Thanks for your answers. Case closed.
I would also add that internal layer footprint support would also be good for high speed production designs. There are plenty of boards that embed 01005 capacitors internally. I have not seen where trenches are made for inductors, but it is discussed here - https://medium.com/supplyframe-hardware/confessions-of-a-pcb-designer-tetris-placement-or-how-to-embed-components-33774457b572
https://medium.com/@tourin.john posts are a great resource on the current state of the art.
A pro tip for DIY experts:
Take a micro usb plug: https://www.ebay.com/itm/10Pcs-Micro-USB-5-Pin-Male-Connector-Port-Solder-Plug-Plastic-Cover-For-DIY-New/192281390466?hash=item2cc4dd2d82:g:iz0AAOSwzaJYAGnW and pry off the plastic part which is is between the solderable pins. You get a nice two-side edge connector for which you can use 1.2mm pcb board, about 10x10mm. I’ve got a two-side footprint if someone happens to need.
Exactly, also edge mount SMA connectors that you slide in.
This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.