In my understanding / language it is a question of what point the kelvin connection is made to.
On a 4-pin/pad current sense resistor it is formed to a point internally in the resistor, which is controlled by the design and manufacture of the resistor and thus presumed (or verified) to be pretty accurate.
On a 2-pin/pad current sense resistor with the PCB layout as you show it, the kelvin connection is formed to the pads on the PCB. This excludes errors from the high current traces on the PCB, but includes errors from the pad/resistor interface, including the solder and connection surfaces on the resistor itself.
This may not be accurate enough for high-precision applications, but as paulvdh says may be a relatively small error in many cases, as the solder connection is fairly low resistance.
So, the best option will be to go for a 4-pad kelvin connection shunt resistor since I am using it for low current and voltages (less than 1A and 5V), right ? Because according to paulvdh and as I understood, 4-pads (terminal) resistors are becoming obsolete.
It depends what level of accuracy you need?
Do you just want to know roughly what the current is, and can allow for a perhaps 1% (guesstimate) error? 2-pad with kelvin connection on the PCB (like your example) will probably suffice.
Or do you need 0,01% (guesstimate) accuracy? 4-pad is the way to go!
Note, you will have to figure out the % accuracy for each option; the values I wrote above are by no means to be taken at face value - I just grabbed something out of thin air for an illustration…
Thank you again for the clarification, actually 1% is enough for me! as I can see in different datasheets, 2-pads connection can provide that precision! So, I will need to buy a 2-pad shunt resistor and do the kelvin connection on the PCB, right ? is there any already available footprints for that ?
Perhaps you should check the Kicad libraries yourself.
If there is a suitable footprint that matches your data sheet, use it. If not, modify the Kicad footprint to suit or create a new footprint yourself.
That used to be “common knowledge”, but I’m not sure about that anymore. In the video below, @14:57 you see a 4-terminal shunt resistor, but the “sense” pads are shorted with the “power” pads. Keithley probably knows what they are doing (or at least, they did before the company changed name 5x or so)
Rabbit linked to the analog website with a talk about different types of connections to current shunt resistors, but unfortunately this method is not part of the comparison. Their Option C (and also D) is the best they have measured, in both these methods, the kelvin connections are not used as intended but are both shorted to either high current track. And it is also the closest to just using two big pads and tapping of the sense wires from the inside of the same pads. When you have a shunt resistor with a value of 0.5m Ohm and push 20A through it, then lowering the resistance between the pads and the resistor itself is apparently the main goal. Also note that options A, B, and E are around 4% off, and all are too low ??? C and D are the only ones that are within the tolerance of the resistor itself. Also curious that the Top Pad method has such a big deviation, but unfortunately they have not mentioned where on the pad they measured.
I’ve modified the KICAD footprint (the footprint which has the same dimensions as the chosen current sense resistor). is this is the correct footprint in that case ? I’ve used a 0.2mm track!
What for you are doing it?
What is the reason you don’t just use standard footprint?
Are you sure you will not want to change voltage tracks direction closer to resistor than your tracks length?
Do you want to have 4 pad symbol and footprint?
How have you added tracks in footprint?
I don’t see the way to do it (V 8.0.4). I can add graphic lines, but not tracks.
If you want it to have 4 pads you have to add extra 2 pads (small, hidden in track (line) ends). If you then insert correct net-tie specification then you will get correct 4 pad footprint.
Even simpler is to just draw the sense wires on the inside, and then lock some of the tracks so the interactive router does not move them. Using net ties is a bit more theoretically correct.
I am having some trouble understanding why all this has not been cleared up long ago yet. Apparently there are some concepts that are too simple for the people wanting to help, so they overlook it, while OP is struggling with some details.
I’ll try again:
Net ties are separate entities. You add them to the schematic as separate symbols, and you assign footprints to them, just like any other footprint. The footprints for net ties, are just two (or more) pads connected with some copper.
To show an example, the project below is made entirely out of symbols and footprints from KiCad’s default libraries.
The intermediate width tracks are from the net ties. I have placed them in such a way that one pad is on the pad of the SMT resistor, while the other is free to connect a track to.
I am trying to use a 2 pads shunt resistor with kelvin connection!
The reason that I don’t use standard footprint is that there’s no already installed footprint that provides kelvin connection for 2-pads current sensor
why would I want to change the direction in that case ? It’s a 2-pads shunt resistor not 4-pads one.
Is it okey to use 0.4mm instead of 0.2mm tracks in the current sensing wires? I just want to have less resistance for better measurement and precision!
Furthermore, is it okey to have a vias on the voltage part (not on the sensing tracks)? Like in the image below, it won’t be affected by a small resistance ?
Then why you just not do it?
In your first post you showed the solution with standard resistor and since then I can’t find what wrong is in it, that you are insistently trying to do it in different way. Why you not follow the way you showed us in this first post. If there is something wrong (that we don’t see) with this solution than tell us what so wrong is in it that you just can’t copy this in your PCB.
The solution from your first post is in my opinion simple and right and ready to be just used. And as you showed it at the beginning that we all know you know this solution but you are looking for something different. Why, and what for?
In what such resistor would be better than standard resistor that you are trying to define special resistor for it? It is why I asked if may be you want 4 pin footprint to be able to use 4 pin symbol at schematic and then using this footprint have there 4 nets separated but at PCB assembled the 2 pin shunt resistor. But you are saying that not. So I still don’t know any answer on my questions from the previous post.
However you define PCB the copper at PCB would be the same. Copper is not informed that it is part of footprint making Kelvin connection and have to take this into account conducting electrons.
It is completely irrelevant whether the shape of the copper on the PCB comes from the footprint or the PCB design.
I’m sure, if I were doing something like that I would use the same solution as you showed in your first post.
To be more clear: schematic:
and PCB:
DRC is getting extended and improved continuously, but it is also getting a bit overzealous sometimes, and it is not a “smart” system that knows your intention. Ignoring DRC violations is a bad habit you should not go into. If you have a long list of DRC violations you want to ignore, then it becomes very difficult to see whether there are import DRC violations that have to be fixed. You can right click on a DRC violation and then exclude certain violations. KiCad puts these in a separate list (See the [ ] Exclusions checkbox at the bottom), so you can flag them as being ignored on purpose, so you can still see all the other violations without the extra clutter.
For the rest, it does not matter much. I would not use 0.2mm thin tracks unless I really have to. Normally I do not go thinner then around 0.3mm, but I don’t really know where the limit is where “most” PCB manufacturers can easily make the PCB.
In stead of answering that, I urge you to do the groundwork and study the 4-wire kelvin connection stuff until you understand it.
It you build your electronics “knowledge” on just rules of thumb and advise given on forums you will never get very far. You need the understanding part for subjects to really sink in and be able to make your own decisions.
i provided the additional input that request as well as other discussions on this topic.
