How do you route multiple nets (like buses) efficiently in Allegro PCB Editor?

If you want to route multiple nets together in one go while maintaining a consistent spacing, then you can use the Interactive group routing in layout editor, which is routing of more than one net concurrently. You can use this feature when routing a bus with traces that follow the same path and have common physical and electrical rules.

To specify the nets for group routing, select the elements (such as clines, pins, vias, and ratsnests) from which to route either by using the Temp Group option from the add connect pop-up menu or selecting the elements with a window. Routing proceeds from the selected elements.

When group routing, you can change the spacing mode between traces to either 'Current mode', which is the default mode, traces continue at the same spacing with which they started. Or you may choose 'Minimum DRC mode', where adjacent traces are separated by the line-to-line space specified in the applicable spacing constraint set. Traces from the same differential pair traces are spaced by the applicable differential pair gap. Or you may choose 'User-defined' and then enter a spacing value.

Attaching a link which talks about Interactive Group Routing and how it works:
https://ask.cadence.com/ASK/techpub-viewer?xmlName=algroroute.xml&title=Allegro+X+User+Guide%3A+Routing+the+Design+--+Interactive+Group+Routing+-+Interactive+Group+Routing&c_version=25.1&path=algroroute%2Falgroroute25.1%2FInteractive_Group_Routing.html&pageName=techpub-viewer

Request you to please explore this if it may help with your requirement.

If you want to route multiple nets together in one go while maintaining a consistent spacing, then you can use the Interactive group routing in layout editor, which is routing of more than one net concurrently. You can use this feature when routing a bus with traces that follow the same path and have common physical and electrical rules.

To specify the nets for group routing, select the elements (such as clines, pins, vias, and ratsnests) from which to route either by using the Temp Group option from the add connect pop-up menu or selecting the elements with a window. Routing proceeds from the selected elements.

When group routing, you can change the spacing mode between traces to either 'Current mode', which is the default mode, traces continue at the same spacing with which they started. Or you may choose 'Minimum DRC mode', where adjacent traces are separated by the line-to-line space specified in the applicable spacing constraint set. Traces from the same differential pair traces are spaced by the applicable differential pair gap. Or you may choose 'User-defined' and then enter a spacing value.

Attaching a link which talks about Interactive Group Routing and how it works:
https://ask.cadence.com/ASK/techpub-viewer?xmlName=algroroute.xml&title=Allegro+X+User+Guide%3A+Routing+the+Design+--+Interactive+Group+Routing+-+Interactive+Group+Routing&c_version=25.1&path=algroroute%2Falgroroute25.1%2FInteractive_Group_Routing.html&pageName=techpub-viewer

Request you to please explore this if it may help with your requirement.

Thankyou so much it helped...

Hi Electro

By default Allegro can route multiple traces at the same time and preserve the spacing between these traces. The spacing would be setup in the constraint manager. Since you are dealing with DDR it might be a good idea to setup in advance of routing some rules to handle your address busses etc, net spacing, net width etc.

To route multiple traces general edit mode will work fine. Click Etch edit icon, then hold down the left mouse button and draw a box over the pins or nets.
Your traces should appear and can be routed off the pins. When routing multiple traces there are two things to be aware of. Control Trace & Route Spacing.

The control trace can cycle which traces the multi line route will follow. It appears as a white x on one of the traces. When the traces are being routed right click and choose "Change Control Trace". The etch will freeze on the screen so another trace can be selected as the control trace. Simply click the trace you wish to use and continue routing. Play around with it to get a feel of how it works.

With route spacing you can specify the space between the traces. When you route off the pins you should notice that your traces respect the spacing of the pins. Route away from the pins then right click & choose "Route Spacing" , you can specify the spacing or use minimum spacing. Choose minimum spacing, The traces should taper down into a nice bus that respects the minimum spacing between the traces. Again play around to get a good feel for the mechanics.

Sometimes while routing busses to and from IC's it can be a real pain to unwind the ends of the nets so as to get a straight point to point path for easy routing. Allegro does have tools to handle this such as the planner, you could look that up.

Another option is to use is a method kind of like from to in Specctra. What you can do is simply draw in your bus and then connect both ends of the nets to that bus. Ideally one would want to do this early on in the design.

Click add connect. Then right click and choose "Multi Line Route"  Fill in the fields, Quantity, Line Width, spacing etc and just route the etch in. This etch does not contain a net name, but you can route a net to it and from it. Doing this can be handy because you can see visually in advance a good possible path your etch might use. Can be useful for what if situations etc.

Best regards.