Designators on multi sheets - Page 1
Forum section: electronics / general

author: c64
author_rank: Frequent Contributor
timestamp: September 02, 2020, 05:58:42 am
content: Is it possible to have two components on different sheets with same designator?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 02, 2020, 10:15:45 am
content: Sure.In the same project? Without errors (and without suppressing those errors in the project settings)? Not recommended.What is your use case?Tim

author: tszaboo
author_rank: Super Contributor
timestamp: September 02, 2020, 10:46:32 am
content: You probably want to look up "multichannel design", and go from there.

author: c64
author_rank: Frequent Contributor
timestamp: September 03, 2020, 04:40:29 am
content: It's a one project, on separate sheets. I don't want to see any errors or suppress them.If I insert sheet into the top level sheet two times, it appends suffix to each designator. But if I insert only once, nothing is appended, so it's possible to have conflicts.Is where any setting to append suffix all the time? I didn't find any

author: c64
author_rank: Frequent Contributor
timestamp: September 03, 2020, 04:41:43 am
content: Quote from: NANDBlog on September 02, 2020, 10:46:32 amMulti-channel is for including one sheet multiple times, I want to include multiple sheets one time

author: Bud
author_rank: Super Contributor
timestamp: September 03, 2020, 06:55:57 am
content: Quote from: c64 on September 02, 2020, 05:58:42 amWould not that cause confusions at the PCB level once you translate the schematic sheets to the PCB?

author: c64
author_rank: Frequent Contributor
timestamp: September 03, 2020, 07:36:35 am
content: Quote from: Bud on September 03, 2020, 06:55:57 amNo, if they have different suffixAnd they will be in different rooms as well.

author: SerieZ
author_rank: Regular Contributor
timestamp: September 03, 2020, 07:55:55 am
content: Sounds like a regular hierarchical Design to me.Make a main sheet where you place blocks as copies of the one sheet you are talking and later define the annotation (Ctrl + L) with the suffix you want.When clicking on the Schematic which you placed the blocks of looking on the bottom left you can see tabs with the different "versions" (Copy_1, Copy_2... etc) and edit them separately as well if you need some differences in between them.Altium also creates the rooms for you like that.

author: c64
author_rank: Frequent Contributor
timestamp: September 06, 2020, 12:09:29 am
content: Must be my Altium is too old. I can open annotations but there is no option to specify suffix

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 06, 2020, 02:20:32 am
content: Check multi-channel design under Project Options.Tim

author: c64
author_rank: Frequent Contributor
timestamp: September 06, 2020, 03:06:18 am
content: Not many settings, I tried different formats but no luck

author: SerieZ
author_rank: Regular Contributor
timestamp: September 08, 2020, 12:37:58 pm
content: First Read up on hierarchical Design and Annotation because I think my explanation is not very good and you will get there yourself easier...I am not sure your version of Altium limits you in this regard, if you can make hierarchical design you should be able to do this.Create one Main sheet, next create your sheet where you actually put the electronics and drag it onto the Main sheet so it gets to be the Child of the Main sheet.On the Main sheet Place a sheet symbol and set the secondary schematic as its Source.Copy and paste that Sheet Symbol with different _1 termination as designator.Select for Annotation $ComponentPrefix$ComponentIndex.$RoomNameThat should genereate for example R76_1 R76_2 per sheet.Good LuckOn a sidenote I find the Annotation in Altium powerful but not very intuitive.

author: c64
author_rank: Frequent Contributor
timestamp: September 09, 2020, 05:55:01 am
content: Quote from: SerieZ on September 08, 2020, 12:37:58 pmIt works!Quote from: SerieZ on September 08, 2020, 12:37:58 pmSo true ...

author: ajb
author_rank: Super Contributor
timestamp: September 09, 2020, 07:36:49 pm
content: Unique designators aren't required for Sch<->Pcb consistency because everything gets linked by the Design Item ID. As long as those are set correctly everything should work even if every single part has the same exact designator. Although if your DIID links get broken (IE, due to copy and paste) it's a lot easier to resolve if they have unique designators.Another way around the problem is to set starting numbers on a per-sheet basis in your annotation settings. In complicated projects you can set the designators to start at hundreds or thousands with the first digit corresponding to the sheet number so it's easy to find the sheet a part is on just from the designator. Multichannel designator strategies still apply.