BOM Generation from editor sheets

[Lyndsay_Doyle]

Clearly I'm missing something here.
I just added a component change to a colleagues design, who has since left the company.
He has editor sheets with numerous copied sheets below this.
I have struggled with this concept for years but I have been told it's a great feature.
Any help with my understanding of how to correct what Altium is doing with the BOM gratefully recieved.
Previous versions of the BOM appear to have been generated without error. This was from AD17.
I have AD22.
Top level editor sheet (for example) has C11. The sheets underneath are PVM1, PVM2 & PVM3.
When the BOM is generated I get C11_PVM1, C11_PVM2 & C11_PVM3.
Clearly this is not what I want.
What am I missing (Apart from brain cells)?
How do I correct this please?

[ajb]

You're talking about tabs at the bottom of the sch editor? Each of those tabs reflects an instance of that sheet in the project, they're not actually "copies" of the sheet.  So you have one sheet called C11, then there are sheet symbols elsewhere in the project that reference the C11 sheet and have the designators PVM1, PVM2, etc. This is simply how Altium organizes multichannel designs. 

Since there are multiple physical parts for each symbol on the schematic sheet, those all need unique designators, and by default Altium appends the designators of the sheet symbols.  There are a few options in Altium project settings for how designators are constructed. You can also reannotate all of the parts based on the PCB design back to basic R1,R2, etc: https://www.altium.com/documentation/altium-designer/board-level-annotation

[Lyndsay_Doyle]

Thanks ajc for your reply and the link to the Altium site.
I get why Altium has this feature.
I dont have a sheet called C11, I have a component called C11 on the "Editor" sheet.
The tabs I have are called PVM1, PVM2 & PVM3.
In the previous issue C11 was annotated as C85, C86 & C87 in the sheets PVM1, PVM2 & PVM3 respectively.
That's fine all working as it should.
Why then when I up issue the design - now (All Components) have the Editor level annotation with the _PVM1, 2 & 3 extension on. Not just for C11, but all components now have this.
I have a number of heirarchal sheets in the design, and they do the same.
I have previously up issued different designs and I have never seen this issue.
I just dont get why it has done this and clueless how to fix this with out cocking up the already placed board layout with approriate designators.
What I am not going to do is randomly re-annotate and then the PCB layout is all wrong.
Worth noting I have this question on Altiums support page and so far, they have not come back with any answers.

[thm_w]

You can see in ajb's link the options have a suitable naming scheme for your preference:
https://www.altium.com/documentation/sites/default/files/wiki_attachments/322206/Dlg-BoardLevelAnnotationOptions.png

As well as the multi-channel options:
https://www.altium.com/documentation/sites/default/files/wiki_attachments/322206/ProjectOptions_MultiChannel_AD20_.png

There should be no "_$RoomName" or similar at the end.
You should have backups of your existing design. Why it has changed, no idea.

[ajb]

From the 'Board Level Annotation' docs:

Board Level Annotation gives you complete control over the annotation in your project with annotation settings saved in an *.Annotation text file displayed under the Settings\Annotation Documents sub-folder in the Projects panel. Altium Designer manages Annotation files automatically.

It sounds like somehow the .annotation file was removed from the project.  Or maybe the project file was renamed, but the corresponding annotation file wasn't.   If you can find that file, possibly in an old copy of the project, you may be able to add it back in to the project.  But if you've made other changes to the design since that file was lost, things may get trickier. 

But after playing with this, it looks like there's a relatively easy way to solve this, as long as the PCB still has the correct designators.  If you do a PCB -> SCH design update, it looks like it will rebuild the annotation file automatically.  This won't update component classes to reflect the new designators, so you'll need to do a SCH -> PCB update afterwards to handle that, but once you do everything should be back in sync with the old designators.  If you've added any components you will need to do a board level annotate on those (you should be able to pick them out specifically in the Board Level Annotate window to do that).  Depending on what kinds of changes you've made and how out of sync the designators are, it might be simpler to go back to the previous project version, make sure the annotations are correct, and then re implement whatever changes you need.

What I am not going to do is randomly re-annotate and then the PCB layout is all wrong.

Just to be clear, re-annotating should never compromise the layout -- it will of course change the designators, but it won't, like, swap component positions all over the board because the designators changed.  Components are linked by their unique IDs, so as long as those are correct the layout and connectivity are safe.  Worst case, if you can't recover the old annotation file or a version of the .PcbDoc with the correct designators, you could go through the board component by component and manually edit all of the designators, then do another PCB -> SCH, SCH -> PCB update cycle.

[Lyndsay_Doyle]

Hi AJB,
Thank you for your reply.
Unlike Altium who still have not responded to me yet about this.
I have read your reply and that makes total sense.
However, WRT to the annotation file, I up issued the design (project) in the way Altium requires so that all the files are still linked. The annotation file has copied or saved across, (as in the attachment) without trying to analyse line by line I have no idea if it's the same, but it was not lost. It's now called issue 5.
I have not added any new components, I have only changed the value of one resistor from 2M to a 1M. I have not changed any designators - Altium has!
I will try the steps you suggest and post back if this works or screws up.
I already have issue 4 so if it does screw up I can go back to that and start again.

[Psi]

Are you aware of the two different annotation types and menus.
Annotation vs Board Level Annotation

[Lyndsay_Doyle]

WTF. WTF & Triple WTF!!!!
I opened my design this morning and read AJB's reply to my post. I copied the project window to show that I had an annotation file.
I open up the offeding pages of the the design and unbelievably the annotation is correct.
I have done absolutely NOTHING to this since last week when I logged out of Altium in frustration and forgot about it for the weekend!

So I now do not have a problem.
I reiterate - I wish I had never bought Altium.
This job, just changing a value of a resistor should have taken an hour.  Up issuing the design schematics and BOM took three days.
WTF.

[ajb]

Ahhh, that's really annoying when things seem to just stop working for no reason and then just start working again also for no reason! 

Something to watch out for: I think the annotation files need to have the same name as the project.  So if you're creating new versions by duplicating and renaming the project in the file system and then opening them in Altium, it might not immediately find the annotation file, but it might have recreated that file or reloaded it in response to something you did between then and now.  If you duplicate the project in the file system but then rename it in Altium (by right-clicking and selecting 'rename' on the project itself in the project pane) then it should rename the other necessary files automatically.

It might be worth taking an extra copy of your project and doing some experiments with this to see if you can replicate the issue and isolate it to anything in particular in your workflow.