2
\$\begingroup\$

I have been experiencing issues with net ties on altium. I am trying to join my separated analog and digital grounds at a single point (star ground) and I tried creating a net tie component to act as a large joining trace for my GND plane and my separated ground polygons

enter image description here

The green arrows show where I am trying to add the ties. I have a few problems however:

  1. I create them with smd pads, so there is no solder mask on them. I tried messing around with the tie's properties but no luck, I cannot add solder mask to cover the copper!

  2. The clearance between the pads is also an issue. I technically need to short the 2 pads to make the rectangle net tie I want in my pcb library component, so Altium will tell me there is a collision between the 2 pads from different nets once I place it.

How may I correct these 2 issues?

\$\endgroup\$
3
  • \$\begingroup\$ Don't use net ties. Just make them all the same net, GND. Problem solved. \$\endgroup\$
    – user57037
    Commented Dec 11, 2020 at 16:37
  • \$\begingroup\$ @mkeith this doesnt work well when you have vias in your analog ground line, it will link the via to the ground plane. Then you need additional of design rules, which is more error prone IMO \$\endgroup\$
    – JCSB
    Commented Dec 11, 2020 at 20:48
  • 1
    \$\begingroup\$ Sometimes you can arrange things so all the analog GND vias are over the analog part of the GND plane, and the digital GND vias are over the digital part of the GND plane. But not always of course. Maybe you are dealing with a complex layout. Anyway, hope the other answer helped you. \$\endgroup\$
    – user57037
    Commented Dec 11, 2020 at 22:01

1 Answer 1

Reset to default
3
\$\begingroup\$
  1. To do this you create a component with two pads set the type to net tie

enter image description here

Make the paste mask and solder mask with negative widths

enter image description here

Connect the pads with a trace.

enter image description here

Here is a good reference for more tips for creating net ties: Net ties in Altium and how to use them

You'll also need to create net tie footprints for each width you need, so every 10 mils is good up to 100 and then every 50 or so.

\$\endgroup\$
0

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