Footprint with tracks, vias, zones

Last time when placing RFID antenna at PCB I just routed tracks. During that (having router set to Shove) the small wrong move of hand and KiCad found the better way removing my 3 track turns including several vias. So for future designs I am trying to make it as a footprint.
Here is what I want to get at the end:

Seeing some similar discussions I supposed that except to follow net-tie solution the rest will be intuitive but I can’t find right tools to use (I use V 6.0.9).

As first try I used one net-tie footprint and modified it adding two pads (to be my vias) and connected them with ‘tracks’ (as there are no tracks in footprint editor I used Draw a line). Here it is.

When I select two left pads with lines at top connecting them and then right-click I don’t see what I could use to make all of that being one pad.
I tried to use my footprint in PCB:

What is good?
Even pads 1 and 2 of my ‘antenna’ are shorted they can be used in two nets.
What is wrong?
KiCad doesn’t see that pads in ‘antenna’ are connected.
KiCad don’t knows to save clearance between other tracks and my ‘antenna’ wires.

Question 1: What are the key information/functions I didn’t found to use?
When it will be done correct then…
Question 2: Is it possible to add to footprint the filled zone - see the shielding at bottom (blue) of my first picture?

In the Footprint Editor you can right click on a pad, and then select: Edit Pad as Grahpic Shapes from the popup menu:

And that is the only way I know of to add “track like” features to a footprint.

There is an option to Lock items,and this also works on tracks. Another option for within the PCB Editor is to make a group of the tracks:

  1. Create some selection.
  2. Right click, and then from the popup menu: Grouping / Group.

Grouping on itself does not prevent the interactive router from shoving things around, but if you Group your antenna, it’s easier to select it as a group :sunglasses: and then lock all track segments and other parts in that group.

Yet another partial solution is to create that antenna in a separate project, (and group it) and then copy and paste it into your project. It makes reuse easier, and if it’s get damaged somehow you can paste in a fresh copy.

But these are all workarounds. I am not aware of a better way to do it at the moment. The best way would probably be to work with “Design Blocks”, but those are not supported yet by KiCad, and it will probably take a few years or so…

1 Like

I will try it (now it is 1:30 a.m. so not now).

I was routing that antenna around 2 years ago and I had a problem (my antenna was replaced by better one :slight_smile: ) when I was routing it. Later I had no problem with it so I think locking will not be helpful for me.

Idea to be considered, but in the case of antena damage during routing next PCB version I can copy from previous version. I know it will be not so easy as from specially prepared file, but the risk of needing to do it is rather small.
I am only interested in having it as footprint. If I fail to have footprint I will do as before.

I supposed it is possible to do it as footprint. Or at least the tracks without shielding fill.
I want to use in footprint lines as tracks and not to construct them from polygons. If not possible with lines than I will wait for V7, V8,…

I am trying and see no useful tools except ‘Finish Pad Edit’ added to context menu.
How to make several pads and some lines (tracks) be one pad?
I must miss something important.

That is correct, exept from the info bar at the top there are no differences in the GUI.

You can add graphics (lines, arcs etch) to a pad in this Pad Edit Mode, and those graphics become part of a pad. The default way to have multiple pads “act as one pad” is to give them the same pad number. I used both these method in the example below.

I experimented a bit with the Idea (and without attempting to make it pretty) and got quite far in KiCad V6.0.10.

  1. I used “Pad Edit Mode” to extend Pad1 and Pad2 to form the loops on the top layer. A side effect is that Kicad now thinks these pads are very big, so ti shows the text also big. The tracks are also recognized by DRC. There are clearance lines around them.
  2. I used THT pads for the via’s, and gave them the same pad number as the real pads to get rid of DRC violation messages.
  3. I extended the THT pad (No 99) to form one of the loops. This works and it’s now yellow. (I did not bother to further modify layers).
  4. Using pad edit mode to add graphics on the bottom layer did not work. It was not accepted by the footprint editor.
  5. Instead, I drew graphical lines on the bottom, and to stop DRC from complaining I added “net tie” to: Footprint Editor / File / Footprint Properties / Keywords. So all the (red and yellow) tracks on the top are parts of pads, and only the two short sections on the bottom are “net ties”.

I also added a test schematic and drew a PCB. I can now run DRC without it complaining. (8.7 KB)

That you can’t use Pad Edit Mode to add lines on the bottom of a THT pad seems to be a bug in KiCad. Maybe I should file a bug report for that… In this case, the “net tie” trick does also keep the pads from shorting to each other so it’s an advantageous side effect.

1 Like

So simple and I didn’t think of it :frowning:
Preparing to that task I have read (month ago) the whole PCB Editor pdf but ‘Creating and editing footprints’ chapter was there empty.
When entering Pad Edit Mode I thought it is not connected with specific pad but a kind of global mode (my mistake) so I not got an idea that everything I add will be added to that pad.
I had my tracks added before entering Pad Edit Mode and expected that when I will select a pad and them I will find in context menu something like “Make Pad from selected objects” (not Add to pad because I didn’t thought of being in editing this one pad).
As you said that pad numbers became big I remind that I have seen such big number after checking what if I use Grouping. Now I think Grouping is what I was searching for, but I was looking for new function and not expecting that standard Grouping got new functionality.
Thanks a lot - you found what I was blind on.
I asked the question as I planned to ask it when I will be back to work with KiCad. And I am back, but I should do one PCB till tomorrow (not critical, but our PCB manufacturer has promotion tommorow) and I am at stage that I am just defining microcontroller symbol. I’m not sure I’ll make it - I can’t get on that antenna right now.

That was the method in KiCad V5 :slight_smile: so it’s quite logical you were searching for that. It is indeed also not easy to discover how it works in V6.

Take your time, the forum will pull it to the front page if you come back in a few days or weeks.

I have to give up with what I wanted to do but during that work I got into another topic.
In KiCad QFN-40 5x5mm with EP3.8 and Thermal vias there are octagons at F.Paste.
I like them as rounded squares I used at such place have to be smaller to have some distance from holes so octagons are better.
I want make holes in vias bigger so I need to make that octagons smaller. When I double click such octagon I see its Pad size, but it is not true pad size. It is calculated like if the line used to make octagon had width of 0. So changing the line width is the simplest way to modify its size. But I like that all 8 corners are rounded. So the better would be to move that lines than to make them 0 width.
I see that I can edit them manually writing each corner positions but it looks I can’t edit it graphically.
What I plan to check is if I can import octagon made with LibreCAD as pade shape (I used import once to define a board shape composed of 14 arcs and 2 straight lines but it was in PCB).
It is my first use of Footprint Editor of V6. I am surprised that I can’t have y increasing up.
And I have continuous problems (I’m sure it is a bug) that Ctrl+S works only in about 50% of times.
I think you can see it for sure if for footprint you ‘Save Copy As…’ with different name in the same library - than it is marked with star as not saved but Ctrl+S doesn’t work (Windows 6.0.10).
At first I supposed that after I save it once with right-click and Save than everything works but later I noticed that not always. I have a problem with reporting anything as I have V6 at PC not connected to net (so even a version text I have to copy via pendrive) and here I have Win7 so not V6.
Specially to have it solved since about 8 months I have a laptop with Win10 but I didn’t finished to install Win10 there yet :slight_smile: so I never used it.

If you play around with a Pad/Footprint, you will more clearly understand the aspects and parameters to change to get what you want…

I loaded the QFN part and tweaked… some screenshots may help you… below…

1 Like

You’re mixing up a bunch of different subjects in your last post…

First those thermal pads…
QFN-40-1EP_5x5mm_P0.4mm_EP3.8x3.8mm_ThermalVias (Phew, what a name…)

I did not understand what you meant from your desctiption, but it became clear when I saw it on my monitor. Here a screenshot with all exept the F.Paste layer disabled:

Those Aperture Pads are indeed looking quite fancy. Chamfered squares with rounded corners… They are almost certainly script generated. A lot of the footprints from the default libraries are generated by scripts, and looking into those scripts is one possibility.

I think you already found this list of coordinates of the lines:

It may seem impressive at first sight, but if you look closer, there are only two different numbers, because the pad is square and all features are symmetrical!
By just deleting the numbers after the 0.2 you already get bigger chamfers. This looks quite close to what you want.

I found the difference a bit small, so I changed those 0.2mm to 0.18mm and the difference is quite visible on the pad:

After you’ve modified one aperture pad, you can select it, right click and Copy Pad Properties to Default, then select the other 8 aperture pads, right click agan and Paste Default Pad Properties to Selected.

Everything put together, it’s a quite easy edit once you figured out how it works, and it seems pretty intuitive to me.

It is even possible to edit them graphically. For this you just enter the Pad Edit Mode with [Ctrl + E] The pads have a circle (that is the “base shape”) and the octagon as a polyline. I can drag corners with the mouse, but it makes a mess of it easily. (Setting an appropriate grid may help)

But I’d say that changing the numbers directly is an easier method in this case.

Indeed, the “Origins and Axes” seems to be missing for the footprint editor for the properties…

I’m not sure about saving with [Ctrl + S].
If I try to save it in the default library, I get the expected Read Only warning.

For the rest, I suggest you first get a bit more used to KiCad V6, and pay some more then usual attention when you’re saving stuff. Maybe the coin will find it’s place, maybe you find out it’s some kind of bug and then you can file a bug report later.

1 Like

Looks like @paulvdh has you covered so, I’ll just add some screenshots to complete my input…

There is indeed a bit of an overlap. I was already typing for some time before you started responding, and I did not read your response before I finished mine.

2…3 years ago I copied one footprint with pads at corner made of polygon and edited them by editing numbers. There were no such symmetry as here. But you are right - only two numbers and copy into all coordinates and done.

And once more - why I didn’t found it :frowning:
That is what I will probably try to use. First graphically to get about what I want and then rounding numbers obtained that way.

I work at my own library. In some cases Ctrl+S simply does nothing, and in some cases works as expected.

Probably won’t make it before V7 appears and everything from scratch :slight_smile:

100% true :slight_smile:
Today I still don’t know all V6 footprint editor possibilities but I was able to do what I want.

Editing them graphically I changed that footprint to:

I reduced the number of vias. Thanks to that at inner VCC layer I will not have the big hole for all vias but small holes each for one via. Not sure if it is important but for me it seems being better.
I placed my octagons not in the center between vias to left 0.3mm between them.

In my other footprint:

I made octagons little asymmetrical to keep distance from the corner vias.

When 2 years ago I used rounded rectangles my manufacturer had a problems with them. I hope he will not have a problem with octagons.

I don’t like interrupting planes either, I do make small groups of vias which interrupt planes, but I always keep them in small groups (3 or 4 or so).

I saw that quite a lot of thermal via’s in KiCad’s default libraries are 0.2mm, while PCB manufacturers often charge extra for via’s smaller then around 0.3mm. I don’t see any benefit of using such small thermal via’s. I would also prefer less, but bigger via’s.

If your manufacturer does not like rounded octagons, then why not just make the aperture mask round? It’s also easier to design, and the paste will flow anyway.

I have read that via hole should be smaller than 0.3 to not steal tin. I don’t remember if it was < or <=.
But in that footprint I changed KiCad 0.2 to my 0.3. Few years ago the smallest hole I used was 0.4.

Conception worth considering.
In past I used only rectangle SMD pads and rectangle openings at power pads. My thinking evaluated from rectangles through rounded rectangles to octagons now. Round apertures in this place never even crossed my mind but octagons are only slightly larger than circles at the same distance from holes.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.