positional reannotation and multi-channel designs

[aandrew]

One of the things I generally do with any design after layout is complete is to reannotate the board so that the reference designators "flow" nicely from left to right and top to bottom.

This is the first time I'm using the multi-channel feature in Altium. I completed the layout as usual, then reannotated and back-annotated the schematic. It worked in the sense that there were no errors, but I can clearly see that the channels do not have the correct designators from the board. It appears that the last component to be annotated is used for all the channels (e.g. if I have four channels and a diode in the channel was annotated as D11, D22, D33 and D44 on the board, the channel will have D44_1, D44_2, D44_3 and D44_4.

If I recompile the project and update the PCB from schematic, the designators "reset" to D44_1, D44_2, D44_3 and D44_4. It seems that positional reannotation and multi-channel are two incompatible features in Altium.

Has anyone else run into this or perhaps figured out how to resolve it? I've been all over Altium's techdocs and while fairly thorough, there's absolutely no mention of this particular combination.

I should also mention that if I generate a BOM from the schematic, it uses the schematic designators (i.e. D44_1 etc.). If I generate the BOM from the PCB, I get different designators, but I can't include a couple of custom part name/value pairs that I want on the BOM.

I'm using 16.1.12 (haven't updated to 17 yet).

[DerekG]

then reannotated and back-annotated the schematic. It worked in the sense that there were no errors, but I can clearly see that the channels do not have the correct designators from the board.

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).

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. Do not use underscore designators in your component numbering.

[aandrew]

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 edit

Ok. 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.

[DerekG]

Why not? I used periods (.) instead of underscores (_)

Because underscores are added by Altium when you cut & paste components on the board. If you adopt the procedure of not using underscores, you can quickly see if the components were added in the usual way (ie from a component library) or if they are a result of a cut & paste.

The back-annotation works from a netlist that is generated when you save the pcb file. I suspect you simply did not save it after you completed the pcb changes. The back-annotation to the schematic therefore was not updated.

[aandrew]

Why not? I used periods (.) instead of underscores (_)

Because underscores are added by Altium when you cut & paste components on the board. If you adopt the procedure of not using underscores, you can quickly see if the components were added in the usual way (ie from a component library) or if they are a result of a cut & paste.

Excellent reason, thank you!

The back-annotation works from a netlist that is generated when you save the pcb file. I suspect you simply did not save it after you completed the pcb changes. The back-annotation to the schematic therefore was not updated.

Hm, that is possible. I was far too flustered to remember if I did that or not, but with everything I just went through (and still trying to figure out why Design/Update Schematics doesn't seem to work but Tools/Back-Annotate does) I'm still a little suspicious there's something a little weird when dealing with positional annotation and multi-channel designs.

Thank you very much for the assistance and the advice!