Assembly Diagram

[Dr_Marko_Rocznik]

My board manuacturer is still using paper for the girls who populat the components on the board.
He wants the assembly diagram to look like this:

In general I do not place use the silk screen for the components reference, simply because in most cases there is not the space for them.
So the references are on the Fab layer.
In order to see the pads I have to turn coper on.
In oder not to see the tracks and filled zones I need to turn both off.
So far so good, but I can not find a way to print it like this.

Eigther I don’t have pads or I have to have tracks and ground plane.

I know that there is this htlm-BOM, but my populator enforces paper…

Marko

[Naib]

Do you really need the pads?
I also need an assembly diagram to capture all the notes specific to assy but less so for population.

As long as pin1 is marked that in theory should be enough BUT every place has its own process
One possibility is to export the fab and copper pads as svg and merge

[dtreffenstaedt]

With KiCad 9, you can plot pad outlines on the fabrication layers.

Leading to output like this:

[supton]

Is there a courtyard layer that you could turn on, with designator on that or a similar layer, to make the print you want? On a board or two I turned off designators by putting to a different layer and dragging inside of the silk box for the component, then making a print that was usable for this.

Failing a nice/easy solution, could you just make a copy of the project and then delete all tracks/floods? Tedious work that I would not want to do often–but if it’s a matter of unroute all could it be used to make a good paper print?

[albin]

Please give Board2Pdf a try to see if it suits your needs. It’s available in the Plugin and Content Manager.

The result looks something like this:

hackrf-one-Assembly.pdf

[Piotr]

@Dr_Marko_Rocznik

He wants the assembly diagram to look like this:

We used ‘since always’ in our documentation a picture containing elements rectangles and references (second picture with values) on top of grayed copper.
This looks like I showed here:

Creating my first footprint: questions as a beginner

I’m trying to stick to that but as Kicad is not allowing me to have 1 symbol mapped to 2 footprints, You don’t understand. If your element has two connectors but not at cables but at its PCB then they both are ‘one insertion’ so one footprint. I started to assemble SMD myself around 1992 and till now I don’t have microscope. When I started to have to use glasses for reading I have bought a workshop lamp with magnifying glass. I have no space at desk for station so I use: Not needed. I…

and I believe is even better for someone populating components as seeing tracks cen better identify places when there are crowded region.

First what I have checked before making decision to move to KiCad was to find the way in KiCad to get such picture. My conclusion (it was KiCad 4.0.7) was that to get it I have to have references and values at courtyard layer. So all my footprints are defined that way. Those time I had to use Inkscape to get my pictures but with KiCad V8 (or may be even V7) I am able to get it directly from KiCad.
The only problem left is output sheet size (solved by 3 hotkeys in inkscape). See:

Resize page to all what was plotted when plot PCB without drawing sheet....

As KiCad allows (I didn’t tried it) to move texts (selected as needed) at PCB to other layer than it should be possible to move them to courtyard as I have and get pictures like mine. If is it posiible to have pads and not tracks - I suppose it should be possible.