Getting re-started with KiCad

(I will assume this connector is a through-hole part.) If you drafted the footprint correctly you need only one footprint. Both top and bottom pads, correctly aligned and oriented, are included in one footprint. Each of the 100 pads on your connector must be specified as “Pad type:” of “Through-hole”, and the affected “Copper Layers” must be “All copper layers”. Each pad’s “Properties” will look something like this in the Footprint Editor:

(I believe “All copper layers” is the default condition when you specify a “Through-hole” pad.)

If you don’t trust a faceless, superannuated, guy to give you reliable advice in this matter, place one of your footprints on a board - plot an output file (Gerber, PDF, Postscript, etc, as you wish) for both F.Cu and B.CU and see if the pads appear on both layers.


1 Like

What do you mean by this? You can create one pin and make an array, then if needed renumber them quickly. This should take a couple of minutes at most if you know how to do it.

I don’t know what I’m doing. I’m just doing and learning right now. These are the first footprints that I have made. The edge connector has 50 rectangular tabs on each side of the board. I have all the measurements of the pads and the locations. It should not be difficult to make the layout of 50 of the pins and both sides are the same. I think the questions is and probably answered by Dale, how are the distinguished between top and bottom of the board. Apparently each pin’s properties include F.MASK and B.MASK. I should check F.MASK for each pin on the front and B.MASK for each pin on the back. Is tha correct? Thanks Mike

An example that you may want to look at for an example of how this can be done is the BUS_AT footprint in the Connector_PCBEdge library. Looking at the pads, each pad is only on one copper layer, only has the corresponding mask layer enabled, and is pad-type Connector. Because the pads top and bottom are directly over each other, you can only see one side’s worth of pads at a time. Switch your active layer from a front to a back layer (copper layers aren’t selectable as editing layers, so try toggling between F.SilkS and B.SilkS) to see all the fingers, one side at a time.

You may need to communicate with your vendor on the proper way to show the pads, especially if you are opting for a hard gold finish. (You may need to connect all the fingers together with off-board conductor that will be removed by the vendor as a final processing step when the board edge is beveled.) Even if you don’t need to add anything specific to the design for finishing, you will likely have to communicate with your board house because they would normally flag as questionable any copper that close to the milled board edge.

Thanks for the tip. It gives me a toe hold. I figure I’ll try to make two rect pads of the correct size and spacing. Then make the two that are behind them. I’m hoping that I can just copy them to make 48. Then the end pads are a little larger and I make them last. Thanks Mike

It might be a good idea to work through this tutorial session: Tutorial: How to make a footprint in KiCad 5.1.x (From scratch)?

In it i give a lot of tips on how such parts with multiple pads in a regular spacing can be made. (TlDr: array tool and custom grid plus duplicate)

Sounds good. I’ll Try it. THanks Mike

I think I have my foot print made. Why do you need a contour outline around the foot print? Is it for locating the footprint? Also how can I check the footprint for proper size? Thanks Mike.

You may be talking about the ‘courtyard’? I think folks have said it is needed for clearance of pick and place machines. To check size I usually do that from the gerbers and print out at 1 to 1. Since I’m usually doing these as a final check I also have my board outline printed so I can use that to double check the scale is correct.

Explained in great detail in the tutorial. But the too long to read answer here:

  • the outline on the silk layer is to help when manually placing parts. (And for optical checks) This is what is printed on to the board. (typically white ink)
  • the outline on the fab layer is for documentation purposes. (i use it additionally for knowing how large the part is while laying out the board. I disable visibility of silk, but show fab)
  • the outline on the courtyard layer is to ensure that enough space is left for assembly. (It is checked by DRC since version 5.)

I’m still learning the terminology. How much bigger should the courtyard be than the actual connector. I made mine just 5 mils. Is that too small? Mike

I must have missed that detail in the tut. I’ll read it again. My outline is cyan or front silk screen. You mentioned a few others, do I need each of them? Thanks Mike

Well i can not tell you what you need. I told you their function. Now you must decide if you want the features connected to them.

OK, at least I’m aware. THanks Mike

Rene already told the basics. I can add some practical notes which are not binding in any way, just my own preferences or experience.

Don’t draw on Silk layer on top of holes, pads or solder mask openings. Also keep some clearance from edges of holes, pads or solder mask openings to silk. This way the silk on your board is readable and nothing is messed up. After the layout is done I check the silk layer by turning off visibility of other than silk and mask (top) layers. Then I move references to nice places. Then I check with the 3D view, it shows quite nicely if silk is on top of a via. That may also make text or line messy if the size is small.

Use the actual component dimensions for the Fab layer outlines. If you mark polarities of components etc. in some way there in the footprints - pin 1 is already marked in many components in the official library - you can use it also as a chart when manually placing parts. I have even printed it to paper, but it may require resizing when printing. References and values may have to be resized for this.

Courtyard is something which you have to learn by making several boards, unless you follow some generic guidelines. You don’t have to care about +/-0.05mm differences. Very often pick’n’place machines can handle much tighter layout than the official library’s courtyards, but you can’t count on that, and you have to know what kinds of components allow which kind of courtyards. If you solder manually you just have to experiment to know what you can do. You may even learn to do the layout without the courtyard layer at all.

1 Like

Look to me because pick and place machine are operating by suck action, spacing between components aren’t issues. Only if you plane to to reword, and hand soldiering is the problem. And I think if courtyard can be configured base on % of the components high would be very help full. For example, if courtyard is extended 26% of part high from part body + thickness of your solider iron. This should guaranteed you to have an open space of 30 degree (+/-15 degree from straight down to the board) for soldiering without having trouble with surrounding parts (specially the tall one).

Using height would also require knowing from which direction the iron comes. It doesn’t make sense to create large courtyard around, say, a high capacitor, if all other components are 0.5mm high. Therefore the needed courtyard is highly (excuse the pun) contextual.

Using it as guide, not rules will be better than eye bowling at them, don’t you think?
Also don’t you think you will having trouble with small SMD component around the tall cap? It would be very hard after you have that cap installed, and reword small component around it. I think the simple and stupid visual guide still better than nothing or a guessing by looking at the image on the screen.

I’m sorry, I don’t undersand that. But what comes to courtyards, I would just let them be as they are and use existing guidelines when drawing new ones. Then I can estimate the needed room by looking at the 3D view and move the components accordingly.

The problem with height affecting courdyard is that it’s very dynamic, contextual, depends completely on the situation and changes when you move components around. The height of the component itself doesn’t affect its own courtyard at all, it’s the heights of the neighbouring components which affect it. And because it depends on the positions of the components you just can’t draw a courtyard around a component when creating the footprint. Some kind of contextual courtyard would be very different thing and should be created dynamically.

I think you see courtyard differently.

  • point of view by @eelik: The courtyard of the component ensures that this component can be soldered in my process.
  • point of view by @nhatkhai: The courtyard of the component ensures that neighboring components can be soldered.