I did a quick search and did not find this, but it may be something I just am missing, but I want to rename a ground net. I know there are the different grounds available like (GND, GNDA, etc.) but if I attempt to change that to say 5V_RTN, or 3V 3_RTN I cannot it says “Power Symbol value field text cannot be changed”. is this possible? Doing so greatly helps when you have numerous power rails that each have to be isolated.
EDIT: After the first reply I also realized that Power symbols are the same way.
Instead of changing the value field, create new power symbols.
Renaming the field is not enough. The name of the net comes from the name of the pin. So, in the symbol editor, edit the pin and change the pin name.
The pin is a little invisible circle, usually at (0,0).
So if I had 6 isolated power rails I have to generate 6 new symbols. Man this is just painful.
Since I am still semi-new to KiCAD, you comment made me look at the Voltage Symbols. Those are the same way so if we need to change the name of a power rail we need a NEW symbol to. Ever other schematic tool ties that name to the net name of the pin.
I guess that is a work around, but deviates from your typical method of documentation of a design. (IMO). Every schematic I have looked at or done there is a Power symbol with the “net” name assigned to it. In Eagle, OrCAD and Altium, there is a generic power symbol that oyu can change the name to and that changes the net that is tied to the pin. Never had I had to generate a “new” symbol for each power or ground rail.
Example:
In OrCAD, two rails, same symbols all I did was chage the symbol label, and the net on the connected wire changed. less than 10 second change.
I like KiCad very much, it has a lot to offer and its performance to price ratio is also very good.
In an Old KiCad version I had made my power symbols in this way, by making the pin name visible and using that as the only visible text. It worked very well until at some point some a KiCad developer decided to freeze the text, and it did not work anymore.
KiCad currently has 45 power symbols starting with a “+” and 18 starting with a “-”, and 35 others, among which the usual VCC, VDD, and a few GND variants. (But no Vcc and Vdd, which I would have prefered, but having both Vcc and VCC would also be … *&^%$#@!)
The motivation for this was apparently to prevent typing errors in power symbol names. But this is a very weak argument. First, if a designer can not spell a word for a power symbol he’s not worth the job. Second. KiCad has the PWR_FLAG symbols, and if a power symbol has a typo then the absence of a “Power output” is likely to trigger the ERC. Third. I never use many power symbols from the library. It’s much easier to hover over an existing one and press c to copy it. Others also regularly use this trick to get more resistors capacitors and such on a schematic. Copying is much easier than fetching new ones from the libraries.
Another way it bites me is with working with transformers.
There are very few AC symbols and doing something like the screenshot below will short the primary winding.
(P.S: Here in the Netherlands it’s common to treat both wires of the 230VAC power net the same, even though one is neutral and the other the phase. Power plug are designed to fit both ways into their sockets).
Are you sure? I think the reason why the pin name is not visible is simply because the file format demands the pin to be invisible for it to count as a global label. The file format also has no field for controlling the visibility of pin text separate from the pin visibility. It could therefore be that you misremember this (or the file format lost features).
Well lets hope there will someday be a better option than invisible power input pins for declaring a pin as a label.
Pain is not big. I have created some power symbols I use, made my power library with only them and forgot of that problem till some day I will have a need of the new one. Then if it will not be solved to that time I will just create the next one power symbol.
I think developers are aware of this problem but have other, more important things, to be worked on.
@ rene: I’m reasonably sure, but not absolute. Back then I tried some 8+ different PCB programs before settling on KiCad. Some of my old schematic (2014-01-07) seem to have a weird text size for power symbols, and maybe I changed it myself during porting or maybe the “resque” did some tricks in the background. I do not have a KiCad V4 anymore. (Maybe it was V3 back then?) Looking forward seems more important…
I’ve looked a bit around on Gitlab and found at least 3 relevant issues:
So it is on the roadmap for V6. I have not yet checked if any form of implementation has started, although in issue 2361 there already was a patch which was refused because of V5.
I wonder, would a brain storming session here on the user forum be useful?
After that we could make a list from some of the best idea’s and combine that with the gitlab issues as some guidelines for implementation.
My Idea is to use a new electrical pin type for power symbols. I’ll call it “Power label”.
A pin with the “Power label” electrical pin type:
Attaches label name to attached wire.
Can be renamed at will (Also when used in a schematic symbol, This allows for power supplies with multiple outputs for example).
Power labels with same name can be connected (as normal).
Power labels with different name is ERC error.
Nets with only one Power label generate an ERC warning.
RefDes decides whether it is a real symbol in the usual way. (for example small isolated SMPS modules)
@paulvdh Completely agree with what you suggested, as long as it carries to ground symbols as well. I have no problem with having different “styles” of power and ground to reflect different “types”, but the simple ability to change the name and have it reflect on what net it is IMO would be great. I have moved over to KiCAD for all by hobby stuff, and with me spending more time at home now due to what is going on I am one it most evenings.
