I moved to Kicad 7 from 6 and i saved this new design as KICAD 7 design ,even generated the netlist from my pervious design and imported here but for some reason my netlist is not showing up here.
Anyone have any idea why?
1 Like
Is Kicad 7 showing any error message?
Pervious? That’s … probably a different word 
And what do you mean with “generated the netlis”? Generating a netlist has been obsolete for 4 years or so.
I’m guessing you have some problem with the assignments from nets to net classes. This has changed quite a lot in KiCad V7. It is now the intention to do this in the schematic (Schematic Editor / File / Schematic Setup / Project / Net Classes and there you can create the net classes and use patterns to assign nets to a net class.
You can also add a “Net class field” to a label by editing the label properties.
A third method is to use Schematic Editor / Place / Add Net Class Directive to add these directives directly to wires.
Ok so i made a new design so i was expecting netclasses to be automatically generated like this in picture from Kicad 6.
but this is not the case so i am confused why this is happening.
No none i opened a entirely new design same issue
Im having this same issue as mentioned in this post.
I have Kicad 6 and 7 both installed and having issues just with Kicad 7
1 Like
Read my previous post again.
The way net class assignments work have changed in KiCad V7, and linking to a KiCad V5 post is useless in this case.
In 7.0 the right-hand box displays the list of nets matching the pattern selected in the left-hand box.
You have no patterns defined, so nothing appears in the right-hand box.
Netclasses in 6.0 were statically defined. Netclasses in 7.0 are dynamically assigned (newly created nets which match a pattern will inherit the netclass specified by the pattern).
Let’s say you had nets 5V+, 5V-, 220V, and CLK. You might use the pattern 5V* to assign the netclass SECONDARY and 220V* to assign the netclass PRIMARY.
Since CLK doesn’t match any of the patterns it would inherit the netclass Default.
Ok, I understood the logic. There are 2 options for setting up circuits.
- You can put a directive and set the Netclass.
- You can group similar nets[!!! Only Global Names, Not Net Labels] (by name) with a pattern and set the class of this group of nets.
2.2 You can also enter all the nets [!!!With Global Labels] and set their netclass, but it turns out you have to enter all the nets manually from memory…(Static linking)
Is there a description of the pattern syntax somewhere? Won’t there be a list of all circuits in the editor?
Where can I see a table of all nets and netclass affiliations?
P.S. Illustration of some relationships.
The pattern will accept either strings with wildcards (*), or regular expressions.
A single wildcard won’t match auto-generated netnames, but something more specific (such as “Net-*”) will. It’s still not a very good idea as the assignment of auto-generated nets can change in unpredictable ways as the schematic is edited.
We don’t have this as the thought was that you’d want to see it graphically. So you can style the schematic (as you’ve done with thick and thicker), and there are even more options in the “Nets” tab of the “Appearances” palette in the PCB Editor (where you can show/hide nets, give them colours, etc.).
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.