Altium Designer 15 - inconsistencies with schematic and PCB synchronisation

[nurega]

I have updated an 'old' design that was originally created using the summer '08 release of altium designer. The project compiles with a few warning related to IO ports and pins, which make little sense (xxxx contains IO pin and output sheet entry objects). I retained the critical aspects of the old PCB, the outline and connector positions, and removed everything else, manually. Then I updated the PCB with the (substantially) revised schematics. 98% of it seems OK, but there are a few very strange things. Some of the components / nets bear no resemblance to the schematic. designators are all OK, I have checked and confirmed, no duplicates etc. there are capacitors in the schematic that show as unconnected in the PCB, with capacitors of other designators showing as being connected to the nets in question, when they are connected elsewhere in the schematic.

Other oddities -

every time I compile and update, there are changes, even if I make no changes in the schematic
in the same update, certain parts are removed AND the same ones added again!

I have tried resetting all designators and re-annotating, but that makes a real mess of the PCB, which is 90% placed (but not routed)

I have spent all day trying to (a) clear all the warnings, just in case they are related and (b) find a workaround for the relatively few parts that are confused vs. the PCB, but without success.

anyone else had a similar experience?

Any ideas how I can get over this without starting from scratch (Im pretty sure the issue relates to updating an old design)

thanks in advance for your advice

 

[Romansh]

Hi,
Have you tried to reset the Unique ID of the problematic components?

 

[ftsolutions]

^- This indeed could be at least part of the problem, especially if you had some composite parts (such as separate inverter gates represented in the schematic) for a single HC04. Another issue could be related to copper pours/polygons that may have been assigned to a net and used to connect pins on the net, instead of distinct traces. Alot was changed over the intervening ~8 years of Altium releases, some things are more effort to bring forward.

 

[nurega]

Thanks for the advice guys. In fact, the issue appears to have been caused by tiny remnants of copper on the PCB (slithers hidden under pads etc.) assigned to nets that no longer exist in the new schematic. Seems that doing so many changes is often troublesome in Altium. The problem was solved by using Design -> Nets -> Clear all nets in the PCB editor. Thereafter all strange phenomenon disappeared!