edit - I don't know what changed (perhaps I recompiled once again?) but now all the channels have correct (from board placement) designators. I'm confused but happy.
edit edit - Ok. WTF.
back-annotate (using the .WAS file) and it says everything's fine, but all the designators in the channels are the same but with different suffix (e.g. D44.1, D44.2, D44.3, D44.4). Go to PCB and Design/Update Schematics. Nothing LOOKS like it's changed, but if I go to a channel page and look at the (CH1, CH2, CH3, CH4 at the bottom I see the part designators are now correct (i.e. they match from the PCB, say D11, D22, D33, D44).
If I generate a BOM from the schematic now it seems to do the right thing. I see D11, D22, D33, D44.
So the confusing parts...
1. Why does Tools/Back-Annotate change all the designators but still show the wrong designators for components in channels?
2. Why does Design/Update Schematics from PCB view not appear to do anything but fix the designators for components in channels?
3. What exactly is the difference between Design/Update Schematics and Tools/Back-Annotate?
I assume that Design/Update Schematics would do more things than just designator updates, but the fact that none of the schematic pages appear changed (no * in their tab) is confusing.
edit edit editOk. I think I have it figured out. See
https://www.eevblog.com/forum/altium/two-designators-on-the-one-component-wtf-!!/ which led me to
http://ludzinc.blogspot.co.uk/2014/08/altium-multichannel.html. TL;DR:
1. (re)compile the schematic
2. Tools/Annotate Compiled Compiled Sheets
3. reannotate from the PCB
4. Design/Update Schematics (from PCB), accept ECO
5. go back to schematic, Design/Recompile
They say that it should be enough, but I found I had to Tools/Back-Annotate and recompile one last time. My designators in the channels are correct, and the emitted BOM is also correct, and I have no more of those D44 (D11) designators in the schematics.
The back-annotation from the board to the schematic has failed.
D44_1, D44_2, D44_3 and D44_4 - these are 4 copies of the part D44 (probably from a copy & paste procedure).
I'm almost 100% certain it did not fail. The Multi-Channel options under project properties are defined as "$Component.$ChannelIndex" (yes, it's a period, not an underscore. Call it transcription error. :-)
You need to go back & carefully look at the Properties of each component. Make sure you change the Designator & not the Comment text, then save the file before back-annotating.
Why would I manually change the designators? My comments are definitely not being changed (e.g. they show correctly as "Schottky Barrier Diode, 2-Pin SOD-123, Pb-Free, Tape and Reel")
Do not use underscore designators in your component numbering.
Why not? I used periods (.) instead of underscores (_) only because I want to use as little space as possible on the silk, but all the Altium docs seem to state is to NOT use nothing (i.e. don't use "$Component$ChannelIndex") and to make sure the character chosen is a valid ASCII character when using the default silk fonts.