Altium designer transfer to pcb issue

Question

I designing a pcb with 14 sheets in hierarchical option. While transfering my components to the PCB doc I get an error sign in some net names without error messages! With that error I get "failed to add class member" error in all sheets and in all signal harnesses.

The second issue that I encountered is in Engineering Change Order when I import the objects and executing. After it, when trying to import the same objects again, without change anything to pcb, some of the objects appear again and still remain in Engineering Change Order, I don't see the expected "no differences detected" message. This disturbs me and I'm afraid for PCB design.

My project, compiled successfully.

Answer 1

The messages should point to specific parts in your schematic. Click on the message and you'll see more in the bottom of the pane. I think "failed to add class member" is usually about parts not having footprints assigned. Project->Component Links... is often the other place to resolve ECO issues having to do with reference designator problems.

Answer 2

I had the same problem where "failed to add class member" prevented the component from being placed on the PCB even though the footprint was properly defined. My work-around was to placed the component manually on the PCB (Home -> Place -> Component) and set the ref des to be the same as the schematic. I then went back to the schematic and updated (Home -> Project -> Update PCB Document) and the error was gone and the netlist updated properly.

Answer 3

Add the library path to the pcb file then the error goes away.

Answer 4

Go into your SCH Library and add a footprint to the part. Recompile the library. Go to your SchDoc and Tools>Updated From Libraries or delete and add the new component back to the schematic and annotate. Go to your PcbDoc Design>Import Changes From

I usually have this problem if I create the part schematic before the footprint and forget to go back to add the footprint before compiling.

Answer 5

It happened to me a few times and in Altium 18 it seemed to be able to manage itself somewhat smarter - I mean the class errors were less persistent than in Altium 19 to me. Anyways, this was my ECO:

Initially I had 3 sets of these 3 errors in both Add Components (Failed to find footprint or so), Add Component Class Members as well as in Add pins to nets sections.

Unfortunately I could not find Project->Component Links in my version 19, but applying Tools -> Update From Libraries and manually reassigning PCB Library paths for all footprints in the Tool -> Footprint Manager only cleared the Add Components errors section.

Indeed, like Devin says, manually placing the component on the PCB and editing its Designator to match the part on Schematic seems to take care of the Add Component Class Members errors. As you can see manually placing component J3 fixed the first error on my list (J3) and 2 errors in Add Pins To Nets section relating to this part as well. This is just a workaround, so would be keen to hear a more elegant way of debugging the class members.

And here is the final run of the ECO > Validate Changes showing a happy sync:

Answer 6

you can select the components from schematic and can go to (part action -> update selected from libraries) then select the footprint manually, this problem occurred to my fiducials which was not showing while pcb placement.....after this works completely fine for me.