Is there an easy way of equalizing the length of the selected Clines? e.g You have a 16 bit data bus and you want to equalize the lengths to 2000 mil (pin to pin)
You could try using constraint manager!
Hello, Please explain. How can i do it using constraint manager? Or Is there any other way? Hope, someone explain it.Thanks.
In the constraint manager, on the relative propagation delay tab, select the nets you want to include in the length matching, and create a match group. In the Pin Delay column, for this group, select longest pin pair. under Relative Delay, Delta:Tolerance, switch from ns to mil. In the Delta:Tolerance box for the nets in your group, type 0:2000. Your group is now set to match within two inches, and a DRC error will be generated for any nets outside this window. Be aware, the tolerance is + or - from the target. Allegro will select one of the nets to be the target, but you can override this by typing target in the Delta:Tolerance column of your selected net. You will then have to set the delta and tolerance for the net selected by Allegro.Regards,Harold
I didn't find the propagation delay tab. Presentily we are using the PCB editor studio version 16.0. Is it available only in performance version? Thanks.
The relative propagation tab is on the left side in the Net folder under Routing.Regards,Haroldharold.email@example.com
Hi, Rules like propagation delay, Diff pairs, match length, area rules are only avalaible in Allegro L w/performance and above. You will have to manually control the length. Or you will have to upgrade. Regards, BillZ EMA Design Automation
Thankyou for all. Especially for AhmetOzsoy for questioned this topic.