I think I have implemented this net tie correctly, and I even think I have used them previously (using older builds) without problem. The rats nest indicates that PCBNew knows what I want, but AGND1 and GND1 zones clear away from my net tie NT1.
Thank you. I downloaded (and thought I had installed) the latest build a few minutes before my post to see if it would fix the problem.
But: It looks like I had maybe re-run the previous build by mistake. I get a version update notice now that open the file after again running the install file
But but: I still see the same issue with the net tie and copper zones. Here is my version information:
OK, I downloaded your project.
I tried manually connecting from the net tie and KiCad complains cannot route from a graphic.
Your net-tie footprint is faulty, it seems to be a graphic symbol
I don’t have your libraries. If I try one of the built in net-ties, I can route from it
Net ties are currently quite hacked together in KiCad, as an artifact that originated in that graphics on a copper layer was not detected by DRC. I assume that the “net tie” keywords were hacked in as a temporary measure when DRC became capable of recognizing graphics on copper layers.
I did a search through de documentation, including KLC (Just a simple text search through various documents) and the string “net tie” is not found in there.
I did know about the “net tie” keywords. I’ve read a few times about them on this forum, and a search brings up 50+ results: https://forum.kicad.info/search?q=net%20tie
Better documentation for net ties is on craftyjon’s todo list:
YeffYoung mentioned that “first class net ties” are pushed to KiCad V7 in:
In this thread eelik posted a snippet from KiCad’s source code which recognizes the “net tie” keyword:
I also looked a bit through: gerber-layer-format-specification-revision-2021-04_en.pdf from Ucamco, and on page 142 there is a mention of an “EtchedComponent”. With (optional) embedded netlists and pad information in Gerber files it’s got all the info in there to do flying probe tests.
I suspected that there might be an issue with my net tie, and I searched FAQ for “net tie” but that did not get it for me. I think I remembered seeing something somewhere about the key word “net tie” and even tried a reference designation of “nettie1” but that did not do it.
If there is some good way to collaborate on an FAQ post I would be happy to contribute and initiate it. But I am 98% certain that whatever I write would benefit from edits by some input from more knowledgeable members of this forum.
I like the “make net-ties first class citizens…” descriptor. As so far as I know, the function has been a “workaround” (one that is widely used in pcb layout tools) for as long as I can remember. In my very limited software wisdom, the idea of including the keywords in the footprint field seems perfectly fine; I suppose that could be extended to languages other than English as need be. To me, this now seems to be less of a workaround than other options I am aware of.
BTW I feel very happy with the idea of putting a net tie into the schematic. It is the documentation realization of (for example) the feedback sense wires for a 200 Amp power supply. You have these 10 mm (guess) diameter ring terminals on the power supply output studs, and they are crimped to some AWG 24 wires for output sense.
It’s an evil, but a nessesery evil. There are a few bugbears of how kicad does them and them becoming “1st class” should improve things.
Right now, I can’t make kelvin connections in a sense resistor footprint. Likewise as they are technically a component, such ties can only go on F.Cu or B.Cu
What naib did in another thread is to use net-ties to make the feedback connections:
I find it hard to believe that an integrated 4 terminal resistor could have a better connection then the much cheaper 2 wire resistor, provided that the connections to the pads are made properly as in the picture above.
[Edit:]
I think it’s part “tradition” from the days of THT resistors. The Kelvin connections became a thing back then, and as long as people keep ordering them, manufacturers will keep making them.
I do have to agree with RobZ’s remark below that parameters in a bought 4-terminal resistor could be more tightly controlled than a solder connection. But how much resistance could there possibly be over the width of an SMT pad combined with both the solder and the metalization of the resistor itself? Maybe it has some advantages for extremely low tempco resistors. Maybe it’s mostly for “habit” and “ease of mind”.
I even saw a video of a teardown with some $$$ equipment which had the four terminal connections on the resistor, but they were just shorted together on the pads. I think it was a Keithley instument and I saw it on EEVblog, but details are vague.
OK…so it sounds like a question of pad spacing violating net class rules? I have wondered whether net class rules are too simple; so that if you have 500V relative to ground but only 1V between two nets, you should not need 500V spacing between those two nets.
On the subject of true Kelvin resistors versus putting 4 or 6 terminals down for a 2 terminal resistor, I think it is a question of mfg control of the resistor construction versus that of your soldering. Getting down to micro ohms and how thick is the layer of fused solder between the pads and the resistor? Are you measuring IR drop in the solder between the pad and the resistor? etc. In theory I would like to think that the manufactured Kelvin resistor is better but I have no data to prove that is the case. I guess that some well controlled soldering with a 2 terminal resistor might be better than a poorly manufactured 4W resistor.
I was reading some of the forum posts about net tie’s a few days ago and created what I think is equivalent to a net tie on an inner layer. To do that though I had to rely on the info of another post that described manually changing the layer in the component file. So, I initially created the pads and graphics on the top or bottom copper layer. Then I opened the kicad_mod file using an editor and changed the layer for those elements that I wanted on an inner layer. When I open the component again in the footprint editor, they appear correctly on the inner layer. I have not attempted multiple inner layers but it appears to work for at least one. DRC runs fine on the component after setting up some custom rules.
