Can you give some example of a potentiometer (datasheet), symbol and footprint which feel problematic to you? Things may be easier to explain with concrete examples.
Thank you for all the help. I have a better grip on it now, I think making my own footprint (and possibly a clearer schematic symbol) is the way.
My main gripe remains, though, but at least now I know that is the way it is supposed to be.
What I think is ”plain wrong” (in my original post) is that the schematic, and how symbols are treated there, is connected to the PCB in an opaque and non-intuitive way. For me, a schematic is a totally symbolic representation of a circuit. I can rotate or mirror a transistor symbol to better fit into the schematic without having to worry how it will end up on the PCB, because that is a representation on a different abstraction level that deals with other things, like the actual board and components. There I can rotate and move the transistor to fit on the physical board.
If I on the other hand rotate or mirror a pot it gets physically different results on the PCB. If I rotate it, as opposed to mirroring it, the outer pins get swapped, which has an effect on the physical world – how a pot is turned.
I cannot fully understand where the difference lies, but one thing is that a pot has a mechanical connection to the user, it kind of reaches across abstraction layers.
Also, the pot symbol has no visible pin numbers in the schematic, and no pin notation in the PCB editor either.
So, I guess I’ll make my own PCB footprint, and possibly also schematic symbol (with pin numbers).
Thank you all!
I still don’t understand. KiCad v5 has symbols R_POT etc. which have pin numbers. The corresponding footprint must also have numbered pads. That’s how all components which are sensitive to pin order are made in KiCad. The symbols can be rotated and mirrored freely because the pin numbering isn’t changed (you just have to draw the wires correctly, of course). Footprints can’t be mirrored. This all is just plain logic, it’s not KiCad specific in any way. So, again, if you can point to the datasheet, symbol and footprint we can explain better if needed.
Edit the symbol with the library editor and, under properties (the cogwheel icon), check show pin number.
I’m sure the pin numbers are there, but not shown.
This is unlikely: every pad of a footprint should have a pin number. There could be exceptions but not for signal pads, for chassis soldered pads in some cases which are not the potentiometer pads.
As eelik says, the link between symbol and footprint are the pin numbers.
As far as I know, all round-knob pots are like this:
Pin 1, down left, counter-clockwise
Pin 2, middle, swipe
Pin 3, down right, clockwise
One footprint from KiCad library:
And the symbol has corresponding pins 1-3 where 2 is the middle one.
All you have to do is draw the wires in the schematic differently according to your application.
I agree. This is explained in detail here: How does KiCad know which symbol pin represents which pad of the footprint?
Footprints can not be mirrored as mirroring a hard body is impossible. (A physical thing can only be rotated and translated. Every other operation can only be done on mathematical or virtual things. A footprint is a representation of a physical hard body and therefore limited to the operation possible on them.)
Might it be that your problem is related with this? https://github.com/KiCad/kicad-symbols/issues/165
Here is the R_POT from v5, it should be unambiguous:
I am on KiCad 4. There are no visible pin numbers on the pot in the schematic – if that had been the case my initial confusion would not have been so big.
I see now that there is pin numbering in Pcbnew, but not that easy to spot (and also, without reference to pin numbers in the schematic, not that useful).
But now I know more, thank you.
The schematic is connected to the PCB by pin numbers. It is predictable and unambiguous (otherwise you would have a hard time designing a PCB). The official libraries provide suggested symbols, you don’t have to use them.
Ah, that may be where you understanding is going wrong. Clearly you can’t rotate or mirror a transistor symbol without it affecting the PCB. Unless you also rotate or mirror the connected wires but that is exactly the same for the pot symbol.
I think all you need is the pot symbol with pin numbers, this was a deficiency that has been rectified in v5.
I’ll try to be clear.
This is a picture of the potentiometer Kicad4 and the settings to show the pin numbers.
As the example with a potentiometer may be confusing, I will use a transistor.
This is the same transistor symbol, rotated and mirrored. I have used letters for the pin numbers. A pin number is actually a 4 character alfanumeric string.
We can see that gate, drain and source are in the same positions.
This is a datasheet of a transistor
See gate is on the left.
Here are 2 foorprints: the real one on the left and a fake one “mirrored” on the right!!
Now you want to solder the chip onto its footprint. So to match the real part to its footprint you must solder the transistor this way:
I hope you now understand why a symbol can be mirrored but a footprint can’t.
It would be not only a bug, but a dead bug.
I hate to nitpick an excellent post, but I think the 4 character restriction has been lifted in v5.
heriks said he is using kicad4…
-You are very finicky
-Well, finicky is not the exact word…
Sorry, I missed that, my bad
In my opinion, with a little extra information, would make a great addition to the FAQs.
One issue that I would like to see added is how the Footprint of the device package affects the pin numbers on the schematic. The physical part defines the pin numbers, and not all transistor packages assign the same junction to the same pin number.
Yes, it can be that fragile, you have many degrees of freedom here.
It is quite easy to get something ‘visual’ on a SCH that is not related to the physical final rotation.
I think the better way to symbolically define a pot, is like Bourns etc do
Notice this symbol has pin numbers and a very clear CW/CCW direction tag too.
The first question that came to my mind, “What happens when it makes physical sense to mount it to the bottom side of the board?”
Yes, and then what happens if the Pot you mount looks like this ?
Hello everyone, especially the KiCad symbol library developers. The following is from IEEE 315, Clause 14.2.5 concerning direction of travel of a rotary pot. Note that it says “…travel viewed from knob or actuator end unless…” What this means is that if a pot is attached to the “backside” of the board CW rotation is as viewing the backside of the PCB and not X-ray view.
IAW IEEE 315, Clause 22.4 that is the “official” list of class designation letters, the class letter R is for any type of resistor, whether fixed value, tapped, settable, or variable. The class letter(s) RV is for a symmetrical varistor or voltage-sensitive resistor–NOT a variable resistor.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.