Author Topic: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?  (Read 4086 times)

0 Members and 1 Guest are viewing this topic.

Offline kandrey89

  • Contributor
  • Posts: 32
  • Country: us
KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« on: December 12, 2016, 08:40:24 pm »
Let's say I have a root sheet, on which I have a child sheet, hierarchy wise, then on the child sheet, I place a GND component among other input and output lines.

Now I know I need to import pins on the root sheet for the child to connect input and output signals, but do I need to do it for GND?

Should I connect GND to a global GROUND label, that seems kind of stupid and wasteful to me, just like bringing out the GND pin onto the root sheet. I realize there might be multiple ground planes, but is that's what Reference and Value is for in the GND component?

Another question, in the GND component, value says GND but Reference says "#PWR?", what does the reference mean with that keyword, is it a macro of some kind?
 

Offline alexanderbrevig

  • Frequent Contributor
  • **
  • Posts: 580
  • Country: no
  • Musician, programmer and EE hobbyist
    • alexanderbrevig.com
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #1 on: December 12, 2016, 09:55:01 pm »
You could easily test and answer these questions yourself. To be honest I have not tested it but I'm fairly certain that a GND in one sheet is a GND in another. You can use other GNDs if you wish, like AGND for analog signals. If you really wanted an entire sheet to have a custom ground reference, I'd say the best way is to use a global label and clearly show how it is connected and at what potential in the parent sheet.

My intuition about the #PWR is used as a hardcoded search term for ERC and maybe also SPICE? I don't know, but if you find out. Share it with the world :)

Offline stryker

  • Regular Contributor
  • *
  • Posts: 78
  • Country: au
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #2 on: December 12, 2016, 10:36:34 pm »
All the power nets are common across sheets.  I presumed it was because the same occurs with all the nets you name yourself, and they're effectively prenamed nets, but I've not actually looked under the hood to add science to that presumption.
 

Offline Bassman59

  • Super Contributor
  • ***
  • Posts: 1140
  • Country: us
  • Yes, I do this for a living
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #3 on: December 13, 2016, 04:25:05 am »
All the power nets are common across sheets.  I presumed it was because the same occurs with all the nets you name yourself, and they're effectively prenamed nets, but I've not actually looked under the hood to add science to that presumption.

Power nets, as defined by placing a power symbol on the schematic, are global, and they inherit the net name from the symbol.  A power symbol GND is global across all sheets, and it is separate from another power symbol AGND.

When you name a net by choosing "Place net name - local label," that net remains local to the sheet. You can also choose "Place global label," which gives that net a global name. Of course you can use hierarchical labels to bring local nets up through the hierarchy to other sheets.
 
The following users thanked this post: kandrey89

Offline kandrey89

  • Contributor
  • Posts: 32
  • Country: us
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #4 on: December 13, 2016, 05:08:48 am »
All the power nets are common across sheets.  I presumed it was because the same occurs with all the nets you name yourself, and they're effectively prenamed nets, but I've not actually looked under the hood to add science to that presumption.

Power nets, as defined by placing a power symbol on the schematic, are global, and they inherit the net name from the symbol.  A power symbol GND is global across all sheets, and it is separate from another power symbol AGND.

When you name a net by choosing "Place net name - local label," that net remains local to the sheet. You can also choose "Place global label," which gives that net a global name. Of course you can use hierarchical labels to bring local nets up through the hierarchy to other sheets.

Thank you, that's very informative. Do you know whether the power nets are defined via the value or the reference? Or maybe the power net is identified via #PWR? Reference and the value serves as the power net's name? In that case, if I change the #PWR? to something else, it will no longer be global, nor a power net.

If I could check I would, but I'm still learning KiCad and not that familiar with all the steps.
 

Offline ElektroQuark

  • Supporter
  • ****
  • Posts: 1206
  • Country: es
    • ElektroQuark
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #5 on: December 13, 2016, 06:27:41 am »
If you edit the symbol, you have a check box to make it a power symbol. It's an intrinsic property.

Offline Bassman59

  • Super Contributor
  • ***
  • Posts: 1140
  • Country: us
  • Yes, I do this for a living
Re: KiCad Eeschema: Are Ground Nets Linked Across Sheets Implicitly?
« Reply #6 on: December 13, 2016, 07:58:45 am »
All the power nets are common across sheets.  I presumed it was because the same occurs with all the nets you name yourself, and they're effectively prenamed nets, but I've not actually looked under the hood to add science to that presumption.

Power nets, as defined by placing a power symbol on the schematic, are global, and they inherit the net name from the symbol.  A power symbol GND is global across all sheets, and it is separate from another power symbol AGND.

When you name a net by choosing "Place net name - local label," that net remains local to the sheet. You can also choose "Place global label," which gives that net a global name. Of course you can use hierarchical labels to bring local nets up through the hierarchy to other sheets.

Thank you, that's very informative. Do you know whether the power nets are defined via the value or the reference? Or maybe the power net is identified via #PWR? Reference and the value serves as the power net's name? In that case, if I change the #PWR? to something else, it will no longer be global, nor a power net.

If I could check I would, but I'm still learning KiCad and not that familiar with all the steps.

The name of the power net is given by the value field in the power symbol. Also, there's a checkbox in the properties dialog "Define as power symbol," which must be checked, and the one pin in the symbol is generally given a name that's the same as the net, and pin number is a ~ character (meaning no pin number).

Finally, the electrical type for that pin is given as "Power input." A power symbol can't be a power output because there would be an ERC conflict if you used the same power symbol more than once in the design, as two outputs can't connect to the same net.

The reference field defaults to #PWR, and after annotation, this will change to #PWR66 or whatever, because each symbol on the schematic needs a unique reference designator.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf