Not really an issue, but just curious as to why?
Using ver 4022 and completed a small board with simple circuit, the power flag and circuit power is labeled as +15V as I have often done in the past.
No other power flags present.
When completing the board layout and routing, the power route shows as +5V, not +15V, nowhere in the circuit drawing can I find any notation of +5V.?
If this happened before, I have never noticed it,
As I said it does not make a difference in the end product, just why?
M.
How did you create the +15V power symbol?
The name of the net is the name of the pin of the power symbol. And in a power symbol the pin is somehow hidden because it is a zero lenght pin. The +15V you see is a text that should match the pin name.
Edit the +15V symbol and inside the symbol editor edit as well the power pin. I would bet the pin name is +5V. Modify and save it with +15V.
By the way, 4022 is 2013 version, eight years and two main versions old. Anyway the power symbol behaviour is the same as in versions 4 and 5.
There can be many reasons why a different netname is shown in pcbnew than you expect. One is of course a wrongly made power symbol. For a detailed explanation on how to make one correctly see the last section of Tutorial: How to make a symbol (KiCad v5.1.x). Be aware that while the user interface will look different for you the file format did not change between 4022 and v5.1 so the underlying technology is the same. (It will only change with version 6)
Another possible reason is that you have multiple labels (or power symbols) connected to the same net in which case one of the names will win (the behaviour is unspecified if multiple lables of the same scope are used)
Looks like it may be something like that, although the power symbols cannot be edited?
I used one from the power symbol library
I am using the older version due to XP PC works well for what I do so far.
Max
Well you can at least look at the power symbol even if you can not save it in the same library. If @pedro is correct then it should be quite obvious.
If there is indeed such an issue then you can make your own power lib with the fixed symbol in it.
And if that is not the issue then double check if any of your placed symbols has an invisible power input pin with pin name +5V.
The power pin +15V should have higher precedence than a hidden pin.
But we are dealing with kicad pre-v4 and it could be that precedences were not tje same as in v4 and v5.
@MaxHeadRoom, can you share your project to take a look at it?
The power symbol is implemented by having an invisible power input pin. This is indistinguishable from any other symbol also having an invisible power input pin (like for example the symbols in the logic libraries).
Both would be converted to global labels. And therefore would have the same priority. If you therefore (by accident or on purpose) connect a wire to such a hidden power input pin of some other symbol then you will connect two global labels and only one of them will win.
I did not create the power pin symbol, I used the one that came in the Power library as I have done in the past.
Here is a shot of the pertinent power references.
.
I think that if you want a +15V power flag and one is not available in the library, you probably need to make your own. Typically I would “save as” starting with one from the KiCad library. When you do that, you need to be sure to change the name of the power pin. I have made that mistake.
Looks like that was it!
I looked at the +15VDC power flag using the editor and although the visible label was correct, the hidden declaration for the pin was +5VDC!
Thanks to all
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.