Differential pair matching issue in sch with weird netName: [N00xxx] - [solved] - Page 1
Forum section: electronics / general

author: Auciele
author_rank: Contributor
timestamp: September 22, 2016, 08:53:14 am
content: Hello everyone,i've been strugling with a specific compiler error for days with my altium 10.1377.27009 and couldn't figure what cause it to pop:On my design there are several Device Sheet connected together on a top sheet (hierarchical topology), some of them feature several differential pairs of net properly named XXX_P and XXX_N via netLabbel and each having a "DifferentialPair" parameter set.Because of the topology some of these net have multiple netName, however i took care of using the YYY_P and YYY_N naming scheme on every device sheet and top sheet.Now about the compiler error, i have several of these:Code:Missing Negative Net for differential pair , positive net where  change from one net to another.What bother me here is:- i couldn't find anyhting wrong in my knowing in the process to declare these net as differential pairs- when using the "Compile Error" box to pinpoint these error location, it lead to nowhere (one device sheet having differential pair is displayed but everything on it is fadded white, no highlight). see attached screenshot- the netName  doesn't look conventionnal to me and i couldn't find any of my net having a name like that in the various altium tools and menus i know.- as far as i can tell, in the pcb editor, differentialPairs all seems to be properly registered by altiumDoes anyone had this compile error out there and have a clue about how to fix it? thank you very much.A.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 22, 2016, 01:45:38 pm
content: And when you update to PCB, the differential classes aren't populated correctly?I wonder if it's something like, the parameter sets only apply on the sheet(s) where the net names are being resolved. Which could be random for each net, I suppose. So, spam each level of the design with parameter sets?... Does that change anything??Pretty sure I've had this before but it's been, well, so and so many years since Designer 10, so I forget if I had a solution or notTim

author: Auciele
author_rank: Contributor
timestamp: September 23, 2016, 02:48:38 pm
content: Hello and thank you for giving me your ideas,like you suggested, i tried to add differential pair parameters set everywhere, didn't solve the problem. In fact i have even more error now (same type).interesting fact, compiling on altium 16 doesn't output these errors.this look like a failure to link beetween sheet and/or wire, but why that's a mystery.my current license don't include PCB so i can't answer to your first question yet. as soon as possible i'll try with my teammate who have it (altium 15)EDIT: on A15, the PCB doesn't import diff pairs, and thus while looking at the classes, no diff pairs appears (my apologies if i'm unclear on this part, i'm not used at all to the PCB interface/concept) that will for sure bring some trouble to the project

author: defter
author_rank: Newbie
timestamp: September 27, 2016, 11:40:40 am
content: this is a very common problem. The problem is that the differetial directive symbol doesn't snap properly to the wire. My solution: replace the directives. If it isn't solve it, then try to rewire this segment of the schematic (the diffpair, and place the directives, and netlabels again). This behaviour was corrected in AD16.1.

author: Auciele
author_rank: Contributor
timestamp: October 04, 2016, 10:07:26 am
content: Hello again, time for a little feedback on this behaviourI ended up solving the issue by replacing all of my blanket with the famous "differential parameter set" attached to them by putting these parameter set directly on the net.Quote from: defter on September 27, 2016, 11:40:40 amI indeed had to replace every parameter set but i barely touched the wire nor the net label, so i don't know if i did what you suggested but anyway thank you, it might help other users.