Re-annotate

[PlainName]

I have a Circuit Studio design which compiles OK (apart from whining about a component class set up in the PCB) and propagates the schematic to PCB. But I added a bunch of components so the annotation is somewhat off in the schematic. I want to re-annotate so that the normal top-to-bottom left-to-right convention is retained. Seems simple, right?

OK, so I pop up the annotate dialog, reset all, then annotate and push the ECO. Green ticks all the way, right up until I push the changes to the PC and then there are a handful of nets that can't be resolved automatically. I try matching them up manually (using the printout from the ECO) but even then some aren't resolvable. Nevertheless, I accept that I'll have to re-route three or four tracks so push on. But the end result is that the PCB has  loads of missing tracks and violations! Surely it can't be that hard to just renumber a component!

Is there some trick to this or is it just not practical to re-annotate a design once the PCB is populated? I figured I'd have a go at doing a few at a time - say, just connectors then just diodes, etc - but couldn't find a way. Seems to be everything or nothing.

This is V1.52, BTW. Current but rather old now and still with obvious bugs.

[voltsandjolts]

Net names are related to components names and so schematic netnames have all changed when you re-annotated.
Then you get mismatches when pushing to PCB (which still has old net names).
Clear all net from PCB (Tools > Netlist > Clear all nets), won't affect PCB tracks.
Then import changes from project again.

[PlainName]

Ah-ha! Thanks, I'll give that a whirl.

[PlainName]

Oh, that's even worse

A fistful of components are treated as new and unplaced, possibly because running the ECO causes them to be deleted then added. That happened originally too, but seems to be worse after clearing the nets. Couldn't spot anything obviously common about these. Most, but not all, seem to be the new components, but some new ones are fine.

[voltsandjolts]

After the re-annotate some component and net names may have stayed the same.
After clearing all nets, things may look worse because now all nets have to be updated, rather than just the changes.
It seems there are still problems with component links, so I would clear all nets, compile the project then have a look at pcb Tools > Component Links.
Manually fix any broken links.

I think the trouble started when you added new components and re-annotated schematics completely.
I normally add new components, annotate only those new components, complie and then update the pcb.
Once those links have been established, go ahead and re-annotate the whole schematic (although I normally back annotate from the pcb to schematic).

[PlainName]

I think the trouble started when you added new components and re-annotated schematics completely.

Actually, I chose not to. I added the new components and just annotated those, compiling and pushing to get on with the layout as per your suggested workflow, with the intention of doing a full re-annotate at the end once everything has settled in place. Perhaps that was a bad move

[voltsandjolts]

Is there some trick to this or is it just not practical to re-annotate a design once the PCB is populated?

It is important to compile the project after re-annotating and before pushing changes to PCB or vice-versa. Other than that, no 'trick' I am aware of.

Yes, of course you can re-annotate a design after the PCB is populated. Or back annotate to the schematic.

It seems something has gone awry for you in this instance, I don't know why ...but then I don't know every step you made.

[PlainName]

Yep, I compile before a push. Makes no difference. I just added anther two components, annotated, compiled, updated PCB... no problem. Works exactly as expected. It's just the global re-annotation that's a problem.

...but then I don't know every step you made

Me neither

Not expecting to have to retrace my steps, I didn't keep track. I am learning about CS right now so it's quite probable I've upset it in some way. Generally I check to make sure things are still on-track after I've had a bit of an experiment and if it doesn't look how I expect I revert to the last save. But, of course, I could've metaphorically kneed it in the knackers and there might not be any visible issue until quite some time later.

[voltsandjolts]

Global re-annotation does work, so I'm not sure what the problem is here.
Feel free to message me with a copy of your ZIP'd project directory and I can take a look.

[PlainName]

Thanks. Just knowing that it should work, and there isn't normally any issue, is a big help on the way to resolving it.

[krish2487]

I faced a similar situation earlier...
and this kinda, sorta worked for me..

reset -> push ECO -> annotate all -> push ECO.

That sequence of steps sort of forced the components / net links to be reset..

Just give this a try and see if it works??

[PlainName]

Thanks for the thought, but same thing happens: goes through everything just fine and then when pushing to the PCB, the validate is all green ticks and it's only when I hit execute that it pops up a few red crosses. Of course, it is far too late to be able to do anything at that point.

[PlainName]

I think I am missing something obvious. The problem seems to be that for some components, instead of renumbering (actually, swapping numbers) it is removing the entire component and then replacing it with a new component with the new number. Additionally, or maybe this is part of the same thing, if there is C1 10uF and C2 4.7uF to swap, instead of just saying C1 is now C2 and C2 is now C1, it says C1 is now 4.7uF and C2 is 10uF. The difference isn't immediately obvious but the essence is that it's kept the number and changed everything about the component until it matches what it should be. I imagine that is basically deleting C1 10uF and replacing with C1 4.7uF.

Can't help thinking there is some switch or setting that deals with this kind of thing, but maybe it is the way I added the components originally.

[voltsandjolts]

OK, if swapped designator names is causing issues, you can try re-annotating such that all designators are changed to something entirely new.

You can do this in the "Tools > Annotate > Annotate Schematics..." option.
Set the start index for annotation at, say 200 (or something more than your highest designator).
Tick the box beside the start index to enable it. Then click 'reset all' button and then update changes button. Accept changes (create ECO) etc.
See pic for example.

Compile and push changes to PCB

Now, back to schematic, repeat the re-annotation with the start index disabled.

Components links have a unique ID for association so I don't understand why this is happening in your case but the above might be a workaround.

[voltsandjolts]

Some documentation on component links:

http://documentation.circuitstudio.com/display/CSTU/WorkspaceManager_Dlg-ComfirmCompMatchesForm((Edit+Component+Links))_CS

You can also search for "Altium component links" to get some further info which is mostly applicable to CS.

[PlainName]

try re-annotating such that all designators are changed to something entirely new

Yes, good idea. That keeps popping up at the back of my mind but getting displaced before it gains traction. It has now though, thanks

[Edit] And the links. That'll keep me entertained for the moment.

[PlainName]

And, just like that, it worked. Not the renumber to something totally different x 2 but the page that link was to. For some reason there were a ton of unmatched components. Since they hadn't been renumbered yet it was trivial to match them all using the designator, and once that was done the renumber went perfectly. No idea why that was beyond CS, particularly since it knew everything and even had them all matched just waiting for the 'apply' mouse click for each pair. But there we go.

Thanks very much for persevering and supplying the ideas