emergency altium layout help (deadline comming)

[SArepairman]

https://www.eevblog.com/forum/altium/some-components-keep-being-reset-after-schematic-changes-are-compiled-to-pcb/msg347427/#new

I have a dead line approaching and I need to finish my design. For some reason 38 components keep being repositioned each time the PCB is updated from the schematic. I tried deleting all the offending parts, but even so, when the update is done they are all moved to the default position.
I am verry fustrated because my PCB is almost done but every time I wanna do a little touch up I need to move 38 parts.

The error is specifically
"Failed to match 38 of xxx components using unique identifiers. Do you want to try and match the remaining components using their designators?"

Then the program removes the 38 parts, adds the 38 parts, removes the 38 parts and adds the 38 parts.

I don't know why these 38 parts are different, I tried restarting altium.


What the fuck!

[tszaboo]

On the PCB editor, there is a menu: Project -> component links (shortkey C, K)
Match the designators. This helps 90% of the time, if you did not mess up a multi channel design.
You own me a beer.

[SArepairman]

What do I do if there are components that are not matched?

For instance I have a U13 on the schematic and a U13 on the PCB, but the unmatched components list shows no unmatched U13 in the schematic but a unmatched U13 in the pcb.


I see them both, but the C K menu does not see it my way.

[SArepairman]

oh i see what this mother fucker is doing, I think it matched up parts inappropriately, it matched up U1 and U13 and so on.


Thank you for yoour help

[Psi]

Yeah, that's one thing Altium designer could do better at.

Sometimes when changing multiple things at once AD will get confused when you do the next PCB update (with regard to what matches to what on the pcb). Then you get the unmatched designators message and have to deal with it.
It happens because AD doesn't try to match things up until you do the next PCB update. So if you have changed or moved net/trace A -> B and also B -> A then it isn't sure which way to jump and has to ask you.

I try to limit the number of serious layout changes between each PCB update which mostly gets rid of the issue.
It would be nice though, if the designators remapping window gave more info so you could figure out what was supposed to match what.


(Unless there's some super easy way to fix this issue that im not aware of.
 Altium is full of useful features people don't realise exist until years later )

[free_electron]

This issue arises because you try to do things behind the back of the system. Don't do that !

if you got misery like that there is something wrong with your design:

here is a flowchart to solve this kind of problems

Step 1) check duplicated designators

in schematic : T-A - click the reset duplicates at the bottom , then run the annotate
D- U

Careful as the part designator and sub block can be locked ! the tool will NOT touch those !! even if they are duplicate. It will throw a warning though during the project compile. if you dont get the error panel : V-W-D-E

Step 2 )
flush the netlists :

In pcb editor D-N-C

Step 3.
Sync the internal database links
in PCB :  C-K

trow everything from right pane to left pane by clicking double arrow, then click button at the bottom : Add pairs matched by and make sure designator only is checked.

Anything remaining is missing stuff.

After this do a Save-ALL (F-L) , then do a design update D-U