Any way to define a bus as "equal track lengths"?

[8086]

I'm doing a design with some DDR3 SDRAM, is there a way in the schematic to tell altium that the data/address bus needs to route to equal lengths?

I can do differential pairs but I can't see a way to do a whole 16 bit wide bus...

[T3sl4co1l]

Directive - Design rule - something about net class or bus class.  Then add a length matching rule (can be on schematic as well) for that class.

Tim

[marshallh]

Create a net class, put all the nets in it, and specify length. The former part is done in the SCH editor and the latter part in the PCB editor

[AlfBaz]

Firstly you need to make sure you have a netclass for the group/s. These are normally generated automatically if somewhere on your schematic you lay down a bus (Place bus) and you add a net label that encompasses that group, something along the lines of data[15..0], where data0, data1 etc are net labels for the individual pins/wires

If, for example you wanted to make your data, address and control lines matched and you didn't already have bus's labelled as described above then simply place a bus connected to nothing with a net label including the [...] thingy. You then Place->Directives->PCB Layout and attach it to the bus wire, edit it adding the DRC rules you want.

The names of the control lines are not usually suitable for grouping with [...]. With those you can create a net class as Tim stated with the Place->Directives->NetClass. Double click it and give it a name such as ctrl_bus. Copy it and add it to all the control lines you wish to add to that class.

The only way I know how to add a PCB Layout directive to these (since you cant draw a bus and label it ctrl_bus) is to wire them into a harness and place the pcb layout directive on the signal harness wire

[8086]

Thanks guys. I have managed to do it with a combination of blanket boxes, applying net class to each.