“some nets were not able to be matched”

[kuldeeps]

Please refer to attached document for error understanding which i am facing while PCB design.
Give me solution!!

[Psi]

If you change too many things at once in your sch altium doesn't know what to do with pcb nets that no longer exist.

Eg if you have a diode and a resistor connected together and altium calls this net "net1". You then route this on the PCB so you have a track called net1

 Then you go and change the diode to connect to a transistor and also change the resistor to connect to a led. (So no longer connected to each other)
Now when you go and update this to PCB altium doesn't know what to do with this old net1 track. Should it be the new net for the led or the new net for the transistor?

If you change them one at a time altium wont need to ask.
If you just randomly pick a net to match to you may find some tracks in you PCB with the wrong net that you will have to fix. (They will be colored green, as an error)

[hkBattousai]

Is there a quick solution when it becomes a total mess after a lot of changes? Is there a way of removing all the nets from the PCB and re-import them from the schematic sheet without ruining the previously laid correct PCB traces?

[Psi]

Good question.

I usually don't change a lot between pcb updates, and answer the unmatched net questions randomly, then fix up tracks if needed.
When doing it randomly at least you sometimes get it correct   better than not doing it at all.

[T3sl4co1l]

Tips:

- When making big changes, expect a whole lot of shit to get fucked up.  Reason: Altium generates net names from random components on the net.  Rename the parts (or pins!) and nets change.
- Usually, those changes are fine; whether they get resolved by brute force (old nets deleted, new nets added) or by matching (usually a tedious, manual process), they get resolved and you're fine.  Sometimes the updating takes a while, yes.
- Prevent automatic net renaming by using manually named nets.  These can also be descriptive (i.e., V_SW vs. NetC1_1), which gives you a potential reminder of what that net is, while routing.
- Occasionally, things will get really badly out of sync, and you kind of need to wipe everything.  D, N, N (Design / Netlist / Edit Nets), select all (you have to select all in the list, CTRL+A doesn't do it..), delete.  Import changes and they should all be back, and correct.
- If copper is getting out of sync, you can use D, N, U (Design / Netlist / Update Free Primitives..) to clean it up.  Disclaimer: it doesn't always work the way you might expect, especially if you still have traces and stuff overlapping pads that changed nets!

Altium does things kind of odd, in that copper primitives have a Net property.  Some EDA packages do that, some don't (e.g., Ultiboard always determines connectivity from pads alone).  You can also correct it manually with S, P or S, C or S, S (Select / Connected Copper, Copper Single Layer or Physical Connection) and entering the new net in PCB Inspector.

Tim

[FivePoint0]

I find it helps to do all deletions then update PCB.  Then do all additions and update PCB.

[free_electron]

there is a shorter way.

in pcb editor : D N C . that kills the netlist.

then push from schematic

[Psi]

heh, D N C

Basically you're telling Altium... Do Not Complain

[mengfei]

what i do is just keep pressing next or ok till I get to the ECO & just fix whatever error shows there 

[Psi]

what i do is just keep pressing next or ok till I get to the ECO & just fix whatever error shows there 

Yep, random