FEDEVEL
Platform forum

Marosh , 10-26-2024, 08:01 PM

I'm working on my PCB layout in Altium and encountered a confusing issue. I did an initial import from the schematic, but since then, I've made further changes to the schematic and reannotated the components. Now, when I try to update the PCB from the schematic, I’m getting a bunch of strange errors that I can’t seem to resolve.

Is there a way to completely clear all the imported footprints in the PCB layout so I can start fresh with a clean import from the updated schematic? Any advice would be greatly appreciated!

QDrives , 10-26-2024, 08:31 PM

What have you got on the PCB?
Do you want to delete everything and start over that way?
You might want to check Project / Component links.

Marosh , 10-26-2024, 08:34 PM

Yes i have some footprint on the layout but nothing is routed yet.. so I wanted to delete them in layout using selection and delete but it changed the wiring in schematics

QDrives , 10-26-2024, 08:36 PM

Make sure that "Tools / Cross select mode" is off before deleting in the PCB.

Marosh , 10-26-2024, 08:51 PM

This worked exactly as I needed. Thanks a lot for your help!:) It literally saved few hours and hairs on my head...

Marosh , 10-26-2024, 09:02 PM

Yet the hopefully new import doesnt work 😦 Lot of Failed to add Class member, missing nets etc..

QDrives , 10-26-2024, 09:34 PM

Then in Design / Netlist, there are some menu items you may want to try.
With Edit nets you can remove all nets in the PCB and import again.
Make sure you validate before importing / updating.

Marosh , 10-27-2024, 11:26 AM

Unfortunately still facing this issue:/ When I create new PcbDoc I can import and get only like 1 easily fixable error but I have hard times doing so in current PcbDoc.. I wanted to use current one since I have already defined the rules.

QDrives , 10-27-2024, 03:05 PM

Ok, sometimes you need to update the PCB twice (Update is from schematic to PCB). The errors shown are not uncommon with missing components.
First thing I would do is:
***From the PCB***
- Design / Netlist / Clean all Nets
- Design / Netlist / Clear all Nets
- Tools / Update from PCB Libraries
***From the schematic***
- Project /Validate PCB project ...
- Design/ Update PCB document ...

Marosh , 10-27-2024, 03:27 PM

I have followed your advice. Made import 2 times with accepting the errors and they were somehow clear after the import? The last error that remains is this one

QDrives , 10-27-2024, 03:33 PM

I do not work with supply nets, so have not seen this yet.
For now I would just ignore these.

Marosh , 10-27-2024, 04:21 PM

It probably comes from these warnings:
I wanted to capture the power flow on top sheet but didnt wanted to uses local power ports in project options since then I would need to route GND everywhere..

Marosh , 10-27-2024, 05:59 PM

Thank you again for your help and quick responses! I have really appreciated it:)

QDrives , 10-27-2024, 07:07 PM

The "supply nets" element is a new thing in Altium. In think it was introduced in AD24.