Diff pair gap changed, need to reroute pair? - Page 1
Forum section: electronics / general

author: jeroen74
author_rank: Frequent Contributor
timestamp: July 27, 2016, 08:37:52 am
content: Any trick to force a new gap setting on existing pairs without rerouting it completely?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 27, 2016, 05:56:59 pm
content: Surely that's a contradiction... how can youchange the path of a routewithout it being a reroute?The easiest you can do is probably poke the autorouter, have it adjust those nets/branches. Or poke the traces manually, so the hug-n-push does the work.Tim

author: jeroen74
author_rank: Frequent Contributor
timestamp: July 28, 2016, 09:25:01 am
content: I don't want to change the pathonly squeeze together a bit the two traces that make up the pair (a certain other EDA package can do it, so why can't Altium?). With rerouting I mean using the 'Interactive differential pair routing' tool.Any yes, I'm poking the traces with the push thingy. The only problem is, I have 120 pairs, with net lengths over a meter long on a board of 865 by 550mm.... and if there's a single clearance error in one trace it won't move it and blocks the rest, so I have to fix that first and the source can be very far away. And fixing that error might mean fixing another error somewhere else. I could disable the clearance rule that defines the 0.5mm spacing between pairs, but defeats the whole purpose of the thing.The push thingy seems to create segments that are slightly off grid, usually around the 135 and 45s angles; the clearance errors are sometimes absolutely tiny, like only 3 microns.At this point it seems just laying down all the traces AGAIN is the only way, as it's just takes too long to use the push thingy (which does work wonderful if no errors are present.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 29, 2016, 12:01:35 am
content: I'm not sure other software is able to do it either... maybe something that generally exerts more control over the design itself, like PADS Router (and, probably, most offerings in the order-of-magnitude-higher-cost tier... but, yeah..).Which kind of hints that, like I said... if you can have the autorouter do it... otherwise, yeah...If nothing else, you can turn off blocking by pressing SHIFT+R while routing (cycles route mode, you want push, or ignore obstacles).If you're getting rounding errors (yeah, I know the feeling...), maybe increase it marginally while routing, then drop it afterwards. Silly hack, and doesn't really help once routed, but..Anyways, only useful comment I really have: do you really need to squeeze the traces? If it's about impedance, remember, differential impedance is, for the most part, a silly idea. Edge-coupled traces have low coupling, and are better thought of as two independent traces being routed through the same path length and surrounding environment (so that noise sources induce equally, and cancel out differentially).Which is also a reminder not to leave the common mode floating, but to terminate it if possible, and to avoid gross CM noise sources (like, running over a split plane with the potential for large RF voltages across the gap!).Most e.g. LVDS transmitters have a modest CM source impedance, around 500 ohms, so the transmission line is weakly terminated at either end, so will magnify CM noise by a low Q factor. This is much better than true CCS drivers would manage, so it's not terrible. ECL output impedance is probably on the low side (and tends to have poor CMRR unless used differentially), so would probably benefit from termination.Tim

author: rfbroadband
author_rank: Unknown
timestamp: July 29, 2016, 05:48:23 am
content: In Allegro one would simply specify the new/different gap for this dedicated diff pair, and that's it, it will be automatically updated without using an auto-router. Which tool are you using?

author: jeroen74
author_rank: Frequent Contributor
timestamp: July 29, 2016, 07:31:32 am
content: Quote from: rfbroadband on July 29, 2016, 05:48:23 amThis is the Altium subforum, so.... yeah... I use AltiumPulsonix (also) updates the traces when you change the width/space settings. I guess it creates loads of DRC error on expansion though. Another neat feature in Pulsonix is that you can edit the two traces as one. It was an absolute major disappointment when I discovered that Altium can't do thatand all it does is lay down two traces and from that point on as far AD is concerned it's just two regular traces (except in the DRC system).I managed to get everything neatly lined up with no DRC errors, albeit with some elbow grease. The use of 'ignore obstacles' (noticed that the current mode is not displayed in the HUD when dragging, only when 'interactively routing') is sometimes the only way to break free traces, splitting the segment from the center sometimes helps too.I need to squeeze the tracks... neatness OCD kicking in, despite that the two signal layers are sandwiched between four solid groundplanes and are not visible at all.I'm well aware of the tight vs loose coupling 'controversy'. This PCB connects to another backplane with a Samtec cable which basically is just 2m of 240 tiny, tiny, really tiny coax cables, not 120 tiny twinax cables.This is an existing design, previously done in CadSTAR by an external party, and I only have to revise it with some minor mechanical tweaks and the addition of some fuses. It's a big and expensive PCB, and I don't want to take too much risk by routing the diff pairs loosely coupled. You know, management saying it worked before, why did you, or why do you want to change it etc etc

author: rfbroadband
author_rank: Unknown
timestamp: July 29, 2016, 04:05:39 pm
content: ups Altium child board...sorry :-).Then my comment was much of any help, but if Altium looses the diff pair info after the traces have been placed you are out of luck. I don't know Altium that much but would I would think that such a fundamental structure as a pair of lines could be changed after the traces have been placed with the appropriate ties into the DRC setup...anyway good luck.