Altium rotates and shifts parts when annotating the schematic - Page 1
Forum section: electronics / general

author: electricar
author_rank: Regular Contributor
timestamp: January 19, 2017, 06:00:57 pm
content: Hey folks,everytime I annote the schematic, the analog switch "TS12A44514DR" gets shifted and rotated around. The same happens with one opamp in my schematic. Besides those two components everything is fine.Does anybody knows a solution to this behaviour?Thank you very much in advance.

author: electricar
author_rank: Regular Contributor
timestamp: January 19, 2017, 06:28:18 pm
content: I found out, that every time I annotate the schematic, Altium wants to swap the parts (2-->3 and 3-->2). If I accept this and annotate the schematic again, Altium wants to to do it over and over again.I already tried this tip from free_electron:https://www.eevblog.com/forum/chat/emergency-altium-layout-help-(deadline-comming)/msg347796/#msg347796But the problem remains...

author: tboy
author_rank: Contributor
timestamp: January 19, 2017, 07:39:14 pm
content: This is an error that occurs with nonhomogeneous parts ie when a component has multiple parts with different graphics. I believe the error is best solved in your library but can be fixed in the schematic as well. In my test case I was able to solve the problem by double clicking on each component gate, which opens the properties for the component. You will notice a check box marked "Locked" in the Properties sub-box beside Part x/y. Checking this box will lock the part so it cannot be changed to another part in the component. If you do this in your library you should never see the error again. I hope I explained this clearly enough and it works for you.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 19, 2017, 08:10:34 pm
content: Patient: "Doctor, it hurts when I do this --"Doctor: "Then don't do it!"If you don't want a full annotation, then don't tell it to do a full annotation!(Didn't know you were telling it that? Well, you know how that goes...)Part numbering is fixed, unless you specifically command a re-ordering, or reset designators (which then obviously need to be assigned to something). Sub-part indexes will be reassigned if the parts are tagged as such, or left if not (Lock Part ID).If you don't want parts moving around, go to SCH Filter, enter the query "IsPart", filter, go to SCH Inspector, and tick "Lock Part ID".Tim

author: electricar
author_rank: Regular Contributor
timestamp: January 20, 2017, 10:15:36 am
content: Thank you very much guys! This fixed the problemAnother question is how do you copy components which already have their assigned designator and unique ID?On compilation I get the "unique identifier error".Is there a way to copy components and deleting the designator and resetting the unique ID with one command?

author: kiran_shrestha
author_rank: Regular Contributor
timestamp: January 20, 2017, 11:21:24 am
content: I think this is because the component in your original library (in schlib) file is moved to some other origin, so try moving the component to another new location in schematic library, and update the component in your schematic of project. This thing also annoyed me for a very long time..

author: ajb
author_rank: Super Contributor
timestamp: January 20, 2017, 12:39:42 pm
content: You can reset duplicate designators with Tools > Annotation > Reset Duplicate Schematic Designators (T,A,I). Note that this won't necessarily reset the *new* component's designator, it could reset the old one's.I don't know about the unique identifier error, AFAIK any new component, duplicated or not, should get a new unique ID automatically. You can reset it in the component properties window, not sure there's an easier way.

author: tszaboo
author_rank: Super Contributor
timestamp: January 20, 2017, 03:09:28 pm
content: Quote from: electricar on January 20, 2017, 10:15:36 amIt should get a new ID when copied. There is a setting to "reset sch. designators when pressing pasteing" or something like that. If only shift+drag would create R? type designator instead of R35, R36...

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 20, 2017, 09:00:34 pm
content: The only situation you should find UID conflicts is if you save a copy of the file, make modifications, then add it back into the project. The two files were once the same file, and therefore any components that weren't deleted will retain their original UIDs.Fix UIDs with Tools/Convert/Reset Component Unique IDs.Pasting and adding new components should always reset the UID.The UID is used to link components to the PCB. After resetting UIDs, you should go to the PCB and run Project/Component Links. Match up any pairs you've broken. (If you've renumbered designators in the mean time, have fun with that...)Tim

author: electricar
author_rank: Regular Contributor
timestamp: January 21, 2017, 11:38:00 pm
content: Quote from: T3sl4co1l on January 20, 2017, 09:00:34 pmThank you all, this could really be possible in my case! I'm getting used to Altium's workflow bit by bit. I restored an older version and fixed some things before I made the update into the pcb. Now everything is fine, but in the future I will follow your advice.Do you mean renumbering the whole project would be a disaster? I can imagine that this could be desired after some schematic revisions in which the designators reach a very high number although the component count is much less (e.g. R1xxx in a project with only 400 resistors). How is the renumbering accomplished in this case without losing the connection to the almost finished pcb?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 21, 2017, 11:58:56 pm
content: As long as the UID links are correct, renumbering is fine. If you break links and renumber, you'll have a bad time.You can set numbering by sheet on the Annotation dialog. (Very handy when you have a big circuit with many sub-circuits to organize!)You can do a similar thing with hierarchical design, where the channel index is, say, prepended onto the designator number. So you get C1101, C2101, etc. for the same part (C101 logical) across the design.Tim

author: tszaboo
author_rank: Super Contributor
timestamp: January 22, 2017, 02:05:20 pm
content: Quote from: electricar on January 21, 2017, 11:38:00 pmThere is a component link between the PCB entity and SCH entity. You can change the designator, but you need to update the link. Also, the relation is not 1:1, becuase an opamp might have multiple parts on sch, but only 1 pcb. On the other hand if you have channels, 1 sch entity will yield multiple pcb parts, one for each channel.

author: ajawamnet
author_rank: Regular Contributor
timestamp: January 23, 2017, 01:35:24 am
content: There's also a way to temporarily Lock Part ID's in the Annotation dialog - Just right click on the Sub column shown and on the flyout select "Lock all Part ID"Also note that the way AD sets up sub part order is in the pull down at the top left - Shown Down then Across on these screenshots

author: technotronix
author_rank: Regular Contributor
timestamp: January 31, 2017, 10:28:46 am
content: I agree. This error is occurred due to components found in some other destination.