FEDEVEL
Platform forum

mulfycrowh , 05-06-2022, 10:57 AM

Hi everyone,

I made a lot of projects and I didn't understand the loss of my differential pair classes that sometimes occurred.
I finally understand the trouble.
I need very often to modify the schematic in order to optimize the routing.
If you have already created your differential pair classes and you click on Design > Import Changes from ..., they will be lost.

That's very disturbing!

Did you already notice that ?
Do you have any solution to avoid that ?

Thanks.

qdrives , 05-06-2022, 01:38 PM

Are the classes in the schematic or did you only create them in the PCB?

mulfycrowh , 05-06-2022, 01:52 PM

From the PCB

WhoKnewKnows , 05-06-2022, 06:10 PM

I think what @qdrives is getting at, is that if you establish certain features in the PCB design that are not in the schematic design, when you import changes from the schematic to the PCB, the schematic will overwrite these features. No doubt there are project settings that control what's imported and what's not allowed to overwrite the PCB design, so this won't happen. Meanwhile, it's usually good practice to set these features up in the schematic and have them imported to the PCB with everything else. Other designers who read your documentation will be better able to know what your intent for the outcome of the PCB design.

mulfycrowh , 05-07-2022, 12:58 AM

I thought that creating differential pairs classes was only possible in PCB ?
The purpose is to define USB2, SATA, PCIE Express ... differential pair classes in order to specify width and gap for each class to match the requested impedance.

WhoKnewKnows , 05-07-2022, 07:31 AM

You can create these classes and settings and associate them with the nets in the design, in the PCB editor. But, by specifying these things in the schematic and stackup editor (impedance profiles) this not only causes the classes and settings in the PCB, but also communicates your design intent (the scheme of your design) to people who review your documentation.

I believe, in order to create these classes and settings in the PCB editor and not have them overwritten by transfer from schematic editor, you would have to make changes to the default project settings.

Alternatively, at each import, deactivate deletion of classes and settings you want to keep when the list of changes is shown in the ECO dialog.

Otherwise, practically everything associated with a net or group of nets in the PCB editor that hasn't been directed by the schematic, will be deleted when you transfer from schematic to PCB and accept all charges in the ECO dialog.

Perhaps @robertferanec​​​​​​​ can recommend a video or videos that explains this?

mulfycrowh , 05-07-2022, 08:03 AM

What I have done at present time, just for testing purpose, is to define a Differential Pairs Routing for USB2 that applies to a Query where I declare the pairs involve (see attached).
It is not overwritten when I update the PCB from Schematic.
Thanks for reply.

WhoKnewKnows , 05-07-2022, 09:32 AM

Good luck 🤞

robertferanec , 05-09-2022, 02:08 AM

In the new Altium you can create diff pair classes in schematic. That may be the reason why it is re-writing them.

In Project -> Project Options -> ECO Generation you can set it to Ignore Differences. Then Diff pair classes from schematic will not be transferred to PCB.