routed length bug?

[tonyh88]

Hey there, I'm looking for a kind soul which would be willing to verify my sanity. Either i'm facing a bug or I don't understand something. Using Altium latest version 20.2.6

I'm trying to length match differential pairs. Traces are mostly routed on layer 3 and switch to layer 1.

I first start by length matching everything on Layer 3. No issue so far everything is matched correctly around 3725mil (this includes the via lenght) as can be seen on image1.

The problem happens when I switch on layer 1. Just for a test here I route a short track. I would now expect the routed length to be 3725+ new track length. However, the routed length is now 3716 which is shorter than previously!!! (image 2)

To make the matter even more complicated. If I manually add up the track length of the primitives for this new short track asdisplayed in the PCB panel just below the nets it doesn't add up to the routed length Altium displays.  (image 3)

Any ideas? I tried deleting everything and starting again but exact same behavior.

Is Altium routed length calculation broken somehow?

Thanks!

[Pseudobyte]

I think i might know what is going on.

I did a bit of a test seeing that your board was many layers.

I created a trace on the top layer it's length is 26.889 mil

I added just a via the length is now 28.433 mil

Now i add a trace to the bottom layer the length is now 29.703

Now i removed the bottom trace and repeated with different layers using the same size trace

Via Only: 28.433
L2: 28.266 (LESS than just via !!)
L3: 29.597
Bottom: 29.703

It would appear that Altium calculates distance when you have a via stub to the center of the via (in the z axis)

Neat, I am always learning something new with this tool.

Whether this is a bug or not is up to you. Should not be an issue as long as you do not have any via stubs.

~Bryan

[tonyh88]

ah! Thanks Bryan for that! That is definitely a part of the mystery!

I'll play with that a bit to test further. Something that remains strange is that the + and - line on the same diff pair don't behave the same so there is another factor in there that I still need to figure out.

It would be nice if Altium's documentation was less cryptic about how this is all calculated.

[Pseudobyte]

You may have better luck with xsignals which is how i usually do diff pairs.

[tonyh88]

thanks again! I never used xsignals for diff pair but i'll give it a try next time