Schematic Four Point Nodes

Brief

Schematic four point nodes is a schematic styling mistake which will not be tolerated in WARG schematics and shouldn’t be done in any schematics! The reasoning for what a schematic four point node is and why they should be avoiding is often missed by novice schematic designers so this document is designed to demystify it. If someone has flagged a schematic four point node in your schematic as an issue and you’re confused, you’ve come to the right place! Don’t fear as resolving them is easy and the reasoning is fairly intuitive!

What is a schematic four point node?

This is an Altium wire in a schematic with no Nodes!

Open

This is a wire with a “three point node”

Open

This is a wire with a “four point node”

Note that this is just two nodes crossing and nets A and B will not be electrically connected.

The Altium Reasoning

Now for why schematic four point nodes should be avoided due to a modern Altium quirk.

The following screenshot shows a four point node again, this time I’ve just given them all the same net label to clearly show that these four wires are electrically connected in Altium

I performed a slight modification in the schematic (try and guess what I did though it’s revealed below) and have relabeled the net names to correspond with how Altium would electrically connect things in the PCB.

This should be impossible right ? All four wires visually go into the node so they are all connected right ? Here let me zoom in as much as Altium will let me (this is a hint) and see if these wires are possibly disconnected?

Well now it’s a little clearer, but lets zoom in all the way (something you’d need to do if you didn’t already know something was wrong).

And sure enough we see net B is not connected to net A. How did I do this? A 10 mil schematic grid. Yep that it. Now I’ve heard it said, “schematic design rules should catch this when validating project” or “I’ll see it when I do the PCB” and these may be true especially for simple projects in most cases it is best to avoid the issue entirely. Avoiding using the 10mil or even 50mil grid completely for schematic wires in Altium is another technique experienced designers use to mitigate this concern in addition to avoiding schematic four point nodes.

How do I fix a schematic four point node?

Simply do this:

Now as long as I see the dot I know all these nodes are electrically connected even when looking from a glance. This is essentially breaking a single four point node into two different three point nodes.

Altium has a feature to automatically splay out the four point node though this is generally avoiding since it adds in diagonal lines which may be unclear at a glance.

You may be asking though, can the same issue happen on a three point node ? Well let’s give it an attempt.

When receding a schematic wire in a 10mil grid using a three point node the dot disappears. Even at a distance (not zoomed in) the dot is visually missing and the lines are visually not connected so this issue is much easier to catch.

Next you may be asking what if I just don’t use a 10mil grid ? At WARG (and most workplace environments) we are enforcing all schematic pins and wires must fall on a 100mil grid to increase readability so if this rule is abided by one will never have a problem with this 10mil grid issue. Unfortunately, switching schematic grids is as simple as accidentally clicking the “g” key on your keyboard (assuming default Altium key binds). This could happen to anyone and would be a tragic way to end up with a board that doesn't work.

A visual justification

Another reason to ban four point nodes is they’re ugly and decrease readability. When analyzing the below two examples it is simpler to see what’s going on in the first example than the second because GND symbols are directly connected!

A copying justification

Even if you are not using Altium, or any CAD for that matter, there is still good justification for avoiding four point schematic nodes.

The historical reason for avoiding schematic four point nodes is due to how scanners and printer used to function. Often times your schematic will need to be printed for viewing. You may laugh at this initially, though be aware that when working on certain applications you may not be allowed to bring a computer or be in a harsh environment trying to debug a system. This is less frequent now, but historically schematics were drawn and/or marked up by hand which would then need to be scanned.

With that context let’s take a look at these two separate wires crossing.

With an old school scanner and printer with low resolution, over time if something is scanned and printed over and over again would result in the intersecting lines will build up error/blotching until it appears as though there’s a circle in the middle. Something like:

This will result in confusion when someone is reading the schematic if the dot is actually intended to mean a four point schematic node or if the dot is a result of printing/scanning cycle error building up over time.

Even though your schematic may never be printed keep in mind that this is a longstanding standard in the industry and developing a readable schematic that’s easy to understand is always the goal!