Is label tool always changes the net name? Or only unnamed connection?
Using Kicad 7.99
The label tool’s purpose is to give nets names. So I’m not sure I understand your question. if you put different labels onto the same net, this will create a conflict and one of them wins. The logic which wins is pretty complicated, but power symbols and global labels usually have a higher priority. So adding a label onto the GND net (which has a GND symbol) probably has no effect other than raising a warning.
OK, got it. Thanks.
So I will file a wish list to includes net names priority in the documentation.
However, I still does not understand about power symbol. I connect 2 power symbols, and try change the value of one of them. It may changes the net if wins, but i unsure which wins, the old value or new?
The proper behaviour i think should be:
- Place net label or power symbol will automatically follows old net value, the edit box automatically filed.
- If user changes the value (power symbol) or edit the name (net label), then the net will changed.
- However, this requires scanning around the schematic to change all power symbol values (if shown) and net label which connected to changed net.
Probably random, and changing power symbol values is a new feature in 7.99 that might not be finished completely.
I don’t think it makes sense to connect different power symbols together. What are you trying to do?
In case you want to connect - say - GND and GNDA, you need a net tie.
Hello @sugenganthos
Don’t forget you are using the current development version. Proper behavior of much of 7.99 may not be finalised 'till January next year and changes to anything in 7.99 may occur on a daily basis.
Instead of connect different symbol, I mean more of typo.
Example: Inverter design on the power part may have
GND_Power_U, GND_Power_V, GND_GateDriver, GND_Logic.
The GND_Power_U may wrongly use GND_Power. Then when the designer realize, he would change into GND_Power_U. But renaming many attached symbol may skipped one.
But if renaming one power symbol value can rename all attached net, then it better. (many IDE called this as “refactoring”).
Having different labels or power symbols connected to a new should always create an ERC warning. So you should be able to detect mistakes like that, and it won’t really matter that you get a random or false result.
I understand, but that’s not really how KiCad operates. It just lets you draw whatever you want and the ERC tells you afterwards about possible problems. Automatically relabelling or renaming existing elements can be really dangerous if you for example created a connection that you didn’t intended to. The ERC warning lets you decide if you for example created a short, or just had a typo in a net name.
As a side note, having so many different GND nets doesn’t sound like the best approach. You may have reasons, but I find it usually better to use a single GND net and figure out the layout you need on the PCB side using zone keepouts and so on.
2 Likes
So I will file a wish list to includes net names priority in the documentation.
When a single net has more than one net name, it is a error of the schematic. Don’t do it. Even with a priority list, it will be confusing when someone looks at the schematic, someone will mess up the net names and thing they are different nets.
Here is what i do when a single net has more than one function. For example some net can be have the function OUT, but the same pin may be also used to program the µC, so the secondary function is PGD (Programming Data).
Then i will label the net OUT and only OUT. But i will put a text string next to it with (PGD). The () indicate that this is not the right net.
IMHO this is cleared to read and clear for KiCad what the net is called and what the net does.
The proper behaviour i think should be:
The proper behaviour is not have a net with more than a single name.
But if renaming one power symbol value can rename all attached net, then it better. (many IDE called this as “refactoring”).
You can search and replace in the schematic, either in KiCad directly or open it with a text editor. Pretty easy to change a net name even when it is used at a lot of places.
1 Like
OT: But don’t use 2 different GNDs except for very rare cases. Stick to a single GND is much better from a EMC standpoint. Just keep analog and digital stuff in separate areas with a bit of space in between (GNDs plane should still be fully connected without a gap).
If you place 2 different GND planes and connect them only one a single point, you create a dipole antenna that radiates unwanted which is bad for EMC.
1 Like
Sure. Was meant as an example only. I myself never used split grounds.
Okay, thanks for all advice. And, using more than 2 gnd points sure make a headache.
Also i kind of confuse between functional net vs descriptive label.
The idea of changing net using power pin rename is very useful. Before this, I create 3 gnd symbols with number marker for my project.
I also create the documentation file which is a schematic with many annotations and labels (e.g. pinheader with label for every pin). Maybe plus net label if needed.
It’s documented, see here: Schematic Editor | 7.0 | English | Documentation | KiCad (scroll down to “Net name assignment rules”)
Before this, I create 3 gnd symbols with number marker for my project.
If you have different nets, use different symbols. Important that you can tell exactly what is connected and what not by just looking at a PDF of the schematic.
I also create the documentation file which is a schematic with many annotations and labels (e.g. pinheader with label for every pin). Maybe plus net label if needed.
Why the additional document? Wouldn’t it be better to label the schematic enough so you only need the schematic.
It is the same schematic. That is why annotation or other graphical item is very useful in schematic.
So i overlook this. Thanks for the info.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.