Altium Designer 8: Add netclass in PCB but cann't update sch

Hello,

I am new to Altium designer. I've been trying to add net classes in PCB, Design->Classes.. then Update the schematic but it kept giving the error


Then it shows me the different: "Extra net classes" I choose Update Schematic", create ECO


This is what have in Project Options:

**broken link removed**

Can some body help me with this? Thanks a lot

you can't push net classes from pcb to sch.
the screen you are looking at is from sch to pcb.

Re: Altium Designer 8: Add netclass in PCB but cann't update

So netclasses can only be pushed from schematic to pcb?

I don't see anywhere to add netclasses in schematic though

To add net classes you have to goto
Place>>Directives>>Net Class then you can put that netclass on each of the net which you want to put in a particular netclass.

Similar step you can follow to add as many netclass as you have to use.
I it is not clear please read help file for more clarity

Thanks guys, this kinda sucks since it doesnt have one place like a net class manager for both pcb/schm...

Re: Altium Designer 8: Add netclass in PCB but cann't update

The directives mentioned by Anonymous_Ricky are just parameter placeholders. Once those exist on the schematic, net classes can be pushed from PCB back to SCH. The reality is though, most of the time this is not necessary in my experience.

As for the absence of a "net class manager" - that's not strictly true. Technically net classes don't exist in AD schematics, only directives. The net classes are not generated until you run the ECO from schematic to PCB. Then the net classes exist in the PCB.

From the PCB, there is a class manager, and you've no doubt used it since you created new classes from within the PCB editor.

So... if there was a way to update the class information in the schematics from the PCB, technically, you are only updating the class name placeholders.

Wow, sorry for the long reply there, but I just wanted to clarify how that stuff works a bit more.

Second - if it's just the ECO differences that annoys you, you can modify the ECO comparator options to ignore the extra classes going from PCB to schematic. In your project options, go to the Comparator tab, then find Extra Net Classes and set it to "Ignore Differences".

Let us know if this is helpful or not.

Added after 6 minutes:

Hi iKevin,

One more thing I though worth mentioning - do you use Altium's forums for questions like this?

If you're new to Altium Designer there is really no better place to go - there are lots of experts who've been using the Altium software for years who are very active in helping others get comfortable and efficient with the software. Also the Altium staff and developers are on the forums and can help out.

**broken link removed** if you haven't been there already I highly recommend it.

Of course, edaboard.com is good too ;-) but for Altium specific questions you'll probably get an answer faster on the Altium forum.

Cheers.