Variant changes not shown in schematics nor BOM

I'm almost happy.

In one of my PCB the variant handling works perfectly.

Schematics tells me when a component is fitted or not. BOM shows only fitted components.

Assembly images and the 3D image show me what components are there and what not.

Pick and place file now contain only component to be placed.

But in the 2nd board the "not fitted" components are handled inconsistently.

Two connectors are removed properly everywhere but two "not fitted" resistor are not.

In the schematics they are properly marked as not fitter and they are not listed in BOM.

But in Pick and Place, in 3D image and in Assembly images they are still in-place like the "fitted" components.

All the variants are made exactly the same way. Drawing styles are the same. In schematics Part action -> Variant show these components are not fitter.

The only perhaps related issue is that when I look the properties of a component in Models I typically have "Show" action to show the component footprint.

In the OK board where the "not fitted" resistor is handled properly by the tool there is "Show".

But in the not-OK board the resistors have option "Edit" instead of "Show".

In both PCB projects I use my own schematic and PCB libraries. With the OK board these are links in the project.

With the not-OK board this is local to the project because I made a new component.

So clearly some inconsistency here. And the variants are so close to provide me what I want, so I hope the issues are solved soon. 

Something that may be worth trying. If you have library local and also virtually identical library globally attached then it may be that the system is seeing 'duplicate' components. Does it make any difference to detach the global libraries so that only the local ones are in use?

There is no global library.

The only differences between the projects are that the libraries used in the OK project is in "a library directory" I created when I tried to make an integrated library. This failed and I have started another discussion/question related to that some days ago (no recent progress there).

In the not-OK project these same libraries were copied to the project library and thus used "locally". No other libraries are installed except the CS "standard" integrated libraries that came with the tool installation.

I'll try sometime later if it make any change to move to use libraries in other location than in the project directory.

By 'global libraries' I was referring to those configured under the Libraries... > Available Libraries > Installed. Is there anything configured under Search Path? Just thinking of ways in which the system might be finding duplicate mention of same components.

Sorry, my wording was incorrect. I just consider the installed libraries "global" since they are usable for every project.

No there are on other installed libraries that the Misc Devices and Misc Conn intlibs. There in nothing in the path tab.

In the project tab there is only my own schematic and PCB libraries.

One correction to my earlier post is that the OK project library links point to the libraries local in the other project home directory (the directory where the source files are).

I do not know when this has changed because originally I loaded those existing libraries from the directory I was trying to create the integrated library.

Probably when I moves those same libraries to the home directory of the other not-OK project.

So seems all the components come from the same library and the only difference is the library files are located in one project home directory.

Just a thought, have you tried forcing a recompile of the project and checked the error logs?

From what I can tell, the actual variants are stored in the PCBPRJ file (open it and search for [ProjectVariant1]), and they only become "active" in the schematic and pcb once the project is successfully compiled.

This can be quite confusing when you open a schematic that has variants, select the variant in the drop down and click in the tab that would normally show you the "Physical" schematic instead of the "Design" one and find none of the variants are applied.  If you then go and compile the project everything then starts to work fine.

Edit:

One more thought, the components are references in the variants by designator and unique id, so make sure that in the PCB all the component links are resolved.  I.e. in the PCB go to Tools > Component Links and make sure there is nothing in either of the Un-Matched component columns.

Problem solved! Thanks!

The component linking was the problem. Actually the already "well behaving" connector components were the only one that had matched links. All others 50+ components were paired I guess through their designators. I made all pairs and updated and - Voilà!

Problem solved! Thanks!

The component linking was the problem. Actually the already "well behaving" connector components were the only one that had matched links. All others 50+ components were paired I guess through their designators. I made all pairs and updated and - Voilà!