Sheet level field not passing to footprint

[bertrand_meneroud]

Hi,
I’m using Kicad 8.0.3 on windows.

I have a connector footprint that has a text label called ${ConnName}

I want to populate a different label for each hierachical sheet that use it. So I’ve put a field in the hierachical sheet.
And it does not work. But I’ve already done it with a previous version and it was working so I’m I’m at lost here.

And I have a DRC error saying that it did not resolve the name ConnName

[eelik]

Probably you just don’t remember the details.

This has to be propagated through the symbol. You have to add a field to the symbol and put ${ConnectorName} there. Then you have to use the symbol field name in the footprint text item, so that for example if the symbol field is ConnN, the footprint has text ${ConnN}.

[bertrand_meneroud]

After some testing,
This methode to pass a different name in each different sheet was working before. But It does not work with Kicad 8.0.3.
I can’t remember je version I’ve used where it was working, but I think it was already part of the version 8.0.x

May be I need to do it differently.

[bertrand_meneroud]

Hi,
Yes If I add a symbol field ConnName, I can put a text in it, and I get in the footprint.
But I want a different text for each instance of my connector that I have in different sheet.
And if I change the filed in the symbol, then it change it for every instance of this part.

If in the field I put
Field name :ConnName Value : $(Conn}
and I put a sheet level field called Conn, the variable does not get resolved in my footprint, so I get the text ${Conn}

[eelik]

This is my workflow with 8.0.4:

1. Create a hierarchical sheet.
2. Create a new Field in its properties and give it some text.
3. Add some symbol inside the sheet and add a field to it, using the sheet’s field name as text. Make it visible.
4. Copy the sheet and paste it.
5. Open the pasted sheet’s properties and change the field text.
6. Compare the symbol’s text inside each sheet – it should reflect the different text in the field of each sheet.

Then it’s normal update PCB from schematic, and finally adding visible text to the footprints unless you use a library footprint which already uses that symbol field name in a text item.

EDIT: here’s a project which I used as an example when the hierarchical sheet variables and parameterized sheets were introduced.
hierarchical_sheet_with_parameters.zip (7.4 KB)

[bertrand_meneroud]

I did try your method, and it din’t wokr at first. But I did try it again and it worked, so I must had done something wrong at some point.

May be the way I was doing it before was working in the past, but it was not really supposed to.

Thanks for your help