Altium Designer net classes

[buenos]

hi.

is it possible to define the net/component classes in the schematics level?
if yes, how to do that?

because if i import changes from sch, in the pcb, then it wants to remove all my net classes and component classes. i have to switch off these in the differences list, but if i miss it, then it makes big troubles on the PCB.

 

[House_Cat]

Yes, net and component classes can be defined at the schematic level.

Right click on the project name in the Projects Panel. Select Project Options. One of the tabs is "Class Generation". Check the boxes at the bottom of the page that say "User Defined Classes". Now add your class parameter to the nets and/or components. For nets, use Place>Directives>Net Class. For parts, open the properties for the part and add a ComponentClass parameter. You can also use the parameter manager.

If the ECO wants to remove your classes, it's probably because there is a problem with your component links. You can fix those by going to Project>Component Links from the PCB Editor.

 

[buenos]

@ltium Designer net classes

thanx.

Added after 27 minutes:

this doesnt look good. big balls on a bus.

"04 Feb 2007 22:39 Re: @ltium Designer net classes

--------------------------------------------------------------------------------

Yes, net and component classes can be defined at the schematic level.

Right click on the project name in the Projects Panel. Select Project Options. One of the tabs is "Class Generation". Check the boxes at the bottom of the page that say "User Defined Classes". Now add your class parameter to the nets and/or components. For nets, use Place>Directives>Net Class. For parts, open the properties for the part and add a ComponentClass parameter. You can also use the parameter manager.

If the ECO wants to remove your classes, it's probably because there is a problem with your component links."
-how do you mean?
if the component links window says all components are matched, then?

in the schematics parameter manager, i have tried tried to add this parameter: NetClass to some nets, and add, edit, accept changes, validate... but here it didnt accept my changer, there are red crosses instead of green signs. so i couldnt add the parameter to the nets. this would be better, because this way i wouldnt have to add big simbols to all wires.

 

[House_Cat]

You don't have a choice about using the symbols to designate a net class. You may not like the big red balls, but that's how it's done. If you're not using the directives to assign classes in the schematic, that's why the ECO won't carry them forward into the PCB.

If your component links list is matched - that's good. The problem sounds like it originates from your unwillingness to use the directives symbol. If you don't use it in the schematic, then the only way to assign net classes is in the PCB itself.

 

[buenos]

@ltium Designer net classes

ok. it works now.

but i still think that this is not a too nice solution.
because the shematics will be bigger, and if someone who doesnt know the protel well, and he checks my schematics, he will not understand these things.
And if i have to make a 64bit DDR-DIMM-bus, then everything will be draft full by red circles...

but OK.

 

[House_Cat]

Well, you do have a choice. You can leave the net classes out of the schematic, and assign them manually in the PCB editor (Design>Netlist>Edit Nets). You can then write and use design rules for those net classes - you just won't have documentation for the classes with the schematic.