[SOLVED] Altium: Missing Negative Net

I am getting 3 errors that I cannot locate in my design:

2 look like:
Missing Negative Net for differential Pair [N00674], positive net [N00674]

How do I even find where that is?

One looks like the above, but has a name ,[AMP] and [AMP_P], but I cannot find any breaks or offwire labels or anything that would cause the error! If I cannot find anything myself, how else can I check those lines to find where the problem is?

Thanks.

To define a differential pair on the schematic, you need to do two things:

1) Place the differential pair directive symbol on both lines (positive and negative) in the differential pair. The differential pair directive can be added using the menu Place > Directive > Differential Pair

2) The two nets that form the pair should be named with suffixes _N and _P to denote the negative and positive nets using a net label. You can add a net label using the menu Place > Net Label . (i.e. IFOUT_N and IFOUT_P).

From the sound of your error, I'm guessing that you do not have the differential pair directive symbol added to the negative side of the differential pair. That's what will cause the "missing negative net" error. Also, the net name is currently the N00674 because you have not manually labeled the net. Give the net a label and make sure both nets in the pair have the _N and _P suffixes as well.

That should fix your problem.

- - - Updated - - -

Just in case... here is the link to Altium's help on Differential Pair Directives

cciarleg said:

One looks like the above, but has a name ,[AMP] and [AMP_P], but I cannot find any breaks or offwire labels or anything that would cause the error!

Click to expand...

The negative label is missing its because you have to name the [AMP] as [AMP_N]. This is must for a differential pair.

Look at this video...

I have solved the issue. Just to be clear:

I had differential directives on all the lines. All the lines I could find (including AMP_N and AMP_P) were labeled with a XXX_N or XXX_P net label. Thus the confusion over why the errors were occurring and how to find the nets I apparently missed.

I had one differential directive that was a hair off of the line when I went over all the lines at high zoom. Fixed all 3 errors.

It would be nice if there were a way to see that a little faster-or to see why the other errors happened because of that one item.

Thanks.

Glad you solved it. I try to stick with a 5 or 10 grid when drawing schematics just to limit the chance of a small disconnect occurring. Luckily your minor offset generated an error.

Anyway, if you double click on the particular error and its constituents in the "compile errors" tab, it should zoom/highlight the area of concern, which should at least limit your inspection area and speed up your discovery of the problem. You might have done this, but the slight offset just made it really hard to see what was wrong.

**ALWAYS** set a sane grid for all footprints and also for the schematic and stick to it, makes things very much easier.

Regards, Dan.