How to Clear Existing Footprints in Altium PCB Layout for a Fresh Import?
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.
Use our interactive
Discord forum to reply or ask new questions.