Change designators on SCH without PCB layout changing - Page 1
Forum section: electronics / general

author: bluenote
author_rank: Newbie
timestamp: November 22, 2022, 09:31:44 am
content: Hi,I have a 1800 component design spread across 12 schematics. Each schematic has its designators numbered 1-99, or 100-199, etc. I am now getting close to finishing the design/layout and going through the process of checking the design for error and making design efficiency changes.The upshot of this is that I now have schematics (e.g.) with Q1, Q3, Q5, Q6, Q7. In my simplistic, logical mind, I would have thought that re-annotating this (individual) schematic (so I get Q1, Q2, Q3, etc) would be the way to go.Yes, I can re-annotate the schematic, BUT all of the re-annotated components on the PCB layout get ripped up, put to one side - ready for replacement. Track are left untouched.I spent 2 hours yesterday searching Altium help pages and cannot find a way of simply changing designators without the PCB layout being changed. I'm not changing the actual component. I'm not changing its position on the PCB. I'm not changing its routing. I just want to change designators.Why is this so hard?Does anyone have a method to achieve this?Regards, Bluenote.

author: voltsandjolts
author_rank: Unknown
timestamp: November 22, 2022, 12:02:40 pm
content: Quote from: bluenote on November 22, 2022, 09:31:44 amChange designators in schematic.Net names relate to component names, so compile project to update them.Go to PCB and import changes from project.PCB layout doesn't change, other than designators changing.

author: Psi
author_rank: Super Contributor
timestamp: November 22, 2022, 12:21:15 pm
content: Which version of Altium are you running? I have not had those sort of issues since a really old version of Altium.Also, when trying various methods to fix this make sure you have a backup, it's easy to make things worse.If your running a really old version then what free_electron says in this thread may help to get everything synced back up so thatupdating the PCB from SCH doesn't try to remove and re-add the parts.But make sure you have a backup first!https://www.eevblog.com/forum/chat/emergency-altium-layout-help-(deadline-comming)/msg347762/#msg347762

author: bluenote
author_rank: Newbie
timestamp: November 22, 2022, 01:08:43 pm
content: I do indeed have a VERY old version of Altium 10.For most everything, AD10 works just fine. £9500 for AD22 can't be justified.So, I live with (or work round) its foibles.I'll try the link you gave - and get back to you.Many thanks for your support.

author: voltsandjolts
author_rank: Unknown
timestamp: November 22, 2022, 01:41:17 pm
content: Quote from: bluenote on November 22, 2022, 01:08:43 pmWell, I'm not laughing at that.Thanks to Altium's ever increasing subscription fees, I'll still be on AD22 ten years from now.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 22, 2022, 03:59:41 pm
content: Best guess, your component links broke. Always check them (PCB: Project/Component Links) then synchronize. Then annotation will proceed normally.At least, I think it still worked that way back then.Tim

author: bluenote
author_rank: Newbie
timestamp: November 23, 2022, 11:26:48 am
content: Thanks T3sl4co1l. Thank you so much.That worked - and all is now good.Begs the question though: Why do these links get out of sync in the first place.?Surely synchronisation is buried deep in the inner workings of AD and shouldn't need user intervention.Nor should the end user even need to know how PCB/SCH sync works.[Using a motoring analogy: I don't need to know how brakes work to make my car slow down - only the location of the brake pedal]

author: T3sl4co1l
author_rank: Super Contributor
timestamp: November 23, 2022, 05:04:18 pm
content: Historic reasons, I'm sure.Going back even further, most EDA run/ran SCH and PCB entirely separately, only communicating between them with a netlist or ECO.AD still does this; the update process generates an ECO. The difference is the hacks they added on top of it. The UID for each component gets matched up, and that's how they track updates including designator changes for example.There's no automatic sync, SCH and PCB are always separate; new components are placed with corresponding UID of course, but after that, nothing is done to keep them together aside from Component Links.UIDs are also used for cross probing, selection/highlighting, etc.They can get broken by copy and pasting, various modifications, add/deletion, etc. So it's worth checking from time to time.Hacks, are nothing new, and should come as no surprise; there weren't too many as of AD10 I think, but since then, uh... wait when was multichannel introduced, might already be in there I think... Variants, I don't think do anything funky with UIDs, but variant footprints (AD14-16?? I forget) might, and accordion / length tuning for example is done by special unions of traces (which is one of many kinds of special objects that exist but which you cannot interrogate, so, often lead to inconsistencies and bugs).Tim

author: bluenote
author_rank: Newbie
timestamp: November 23, 2022, 07:35:13 pm
content: Thanks for the insight.Having both PCB layout and SCH capture under one umbrella programme, does lead you into a false sense of security.Especially as a huge amount of info does already pass PCB<<>>SCH when updating.It wouldn't be rocket science for Altium to keep track of changes and synchronise - or even keep a journal of discrepancies (as a prompt for us imperfect humans).My design will have over 2000 components when done and will be around 15-18 months of design, SCH capture, PCB layout and then prototyping.It's an awful lot to keep track of everything - and that's why you pay nearly £10 grand for the design tool.However, from now on, I will treat PCB and SCH as if they were separate applications.You have been most helpful.Again 1000 thanks.

author: Psi
author_rank: Super Contributor
timestamp: November 25, 2022, 02:49:36 am
content: One thing I remember from using really old Altium is that if you do a SCH-PCB update very often it prevents this sort of thing from occurring.The problems tend to happen when you change the SCH parts in one way, then you change them in other way, then you try and do an update and Altium gets confused by all the changes stacked on top of each other.It can track a change of A->B but not when you try to update from A->C because the history of B was lost.So if you do an updated after A->B and another update after B->C then it's fine, but trying to go A->C throws errors.Doing updates often solves the issue, or makes it much more manageable.

author: ajb
author_rank: Super Contributor
timestamp: November 28, 2022, 08:08:44 pm
content: You may also run into situations where a design doesn't compile correctly--there are various conditions in multisheet and multichannel designs that I've seen result in an improperly compiled project, and pushing updates from sch to pcb can in that state can cause additional weirdness. Getting into or out of a weird compilation state can cause component links to be broken, which would result in some of the behavior described in the OP. Actually, this can happen even when the project has been compiling correctly throughout the process if the sheet structure of a multisheet design is changed. Either way it's a good idea to keep an eye on compilation errors/warnings and manually inspect connectivity at a few points to verify that the connectivity on the board matches the intended connectivity in the sch.As far as re-annotating the parts from the board, this is possible using "Board Level Annotation", which specifically allows the designators in the PCB to be different from the designators in the schematic. This is most useful on multichannel designs where you tend to end up with a whole bunch of designators having cumbersome suffixes, which can be changed to simpler sequentially numbered designators. However IME board level annotation is fragile and a big pain in the ass, especially if you try to do it before the design is generally finalized.