3
\$\begingroup\$

I'm learning Altium and trying to re-route an existing board that I have not that much experience with. I've found this checkered pattern in some tracks that Altium is being very annoying at:

enter image description here

They appear by the looks of it when tracks are too close together, if I delete one track it dissapears:

enter image description here

It probably has to do with the fact that Altium does not allow me to place the tracks too close together (0.5mm.) There is no rule that I can see that makes this happen (track to track clearance is 0.15 or 0.2mm,) and when drawing with the clearance boundaries on it doesn't appear to be any restrictions, but I can't place tracks closer than 0.5mm and it doesn't even allow me to place them on the pads of an SMD component because of that.

enter image description here

Both nets are probably a differential pair but I haven't seen any restrictions that apply to that either. Differential routing does not help either, the tracks don't appear (because they would be for sure closer than 0.5mm.) Sorry if the question is obvious, but I've been looking at the documentation for awhile and haven't found anything.

\$\endgroup\$
2
  • \$\begingroup\$ IIRC, this means that one of DRC rules is being violated. But i haven't used Altium for a long time... \$\endgroup\$
    – Morris
    Jul 6, 2020 at 9:18
  • \$\begingroup\$ Yes, that is the first thing i thought, but right-clicking does not show any "Violations" option that shows the DRC violations in other cases. \$\endgroup\$ Jul 6, 2020 at 9:24

3 Answers 3

1
\$\begingroup\$

You can't superpose differential pairs. Altium would show the same error also if you use Interactive routing to draw each wire of the diff. pair instead of drawing both at the same time using Interactive Differential Pair routing.

enter image description here

Also, differential pair are vulnerable to noise on PCB compared to a shielded twisted pair.If you would like to have a protected signal you would have to make a proper DIFF Pair and use a grounded polygon below it.

enter image description here

For example L1 : Diff pairs L2 : Ground plane ..

\$\endgroup\$
1
  • \$\begingroup\$ To the OP, not sure if you are familiar with diff pairs. Look at the pin names ADC_INC_N and _P, that's a differential pair "positive" and "negative" \$\endgroup\$
    – P2000
    Jul 18, 2020 at 1:36
1
\$\begingroup\$

TLDR: Check the Max Uncoupled Length parameter in your Differential Pair Rule.

That pattern is used where a rule can't or shouldn't pinpoint a specific entity causing the error.

In your case, it's most likely the Max Uncoupled Length parameter from the differential pair rule.

e.g. if the signals in your pair are separated for longer than the defined Max Uncoupled Length, Altium won't be able to specifically tell you which tracks, arcs and/or accordions are in error because it could take multiple primitives within the signals to cause the error. So Altium displays the error in a different way, telling you there is something wrong with a portion of the signal path, not just a specific primitive in wrong. When you delete a track, the error disappears because Altium can no longer check the Max Uncoupled Length.

Based on your images, you've tried to route your differential pair with broadside coupling which I don't think you can easily do in Altium. The error will disappear if you correct the routing, or adjust the Max Uncoupled Length. But I think you should correct the routing.

The Parallel Segment rule behaves in a similar way but with more parameters that can error.

\$\endgroup\$
0
\$\begingroup\$

The wires you are placing probably don't have a net name - DRC will complain when you try to connect an unnamed track to a named net.

If you start placing a track from a pad, the new track should pick up the net name, but if you start a track from a random location (even from an existing track, I think) the newe track will not have a net name.

\$\endgroup\$
1
  • \$\begingroup\$ Hi Peter. The net names are ADC_INC_P and ADC_INC_N as shown in the OP images. \$\endgroup\$
    – Dan
    Jul 8, 2023 at 16:43

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.