0
\$\begingroup\$

When connecting a thru hole, via or otherwise, to an internal GND or PWR plane, the default Altium configuration uses a thermal relief connection.

Although I've seen a number of posts saying to abandon thermal reliefs in favor of direct connects, I'd like to try reducing the size of the thermal relief first. The default configuration uses an expansion of 0.508 mm and 0.254mm air gap - leading to overlapping copper pours for vias that are close to each other.

What are the design considerations or reference standards I can use to make sure I don't size them too small?

\$\endgroup\$

1 Answer 1

Reset to default
3
\$\begingroup\$

This depends on the capabilities of your PWB manufacturer.

Most can manufacture down to 0.1 mm (4 mil) space and trace dimensions with no impact on cost. Really low-cost manufacturers might require larger dimensions. If you pay more (or you're already paying more for finer features elsewhere in your design) many manufacturers can do at least slightly smaller.

Also, if you're using heavy copper (more than 1 oz or 35 um thickness) you might need to use larger dimensions.

For a definitive answer, contact your manufacturer.

Edit

In your question you said you're using Altium and in comments you said, "My CAD program doesn't seem to distinguish between vias and TH when forming connections to internal planes." This isn't correct.

In the rule editor, for power plane connections, if you choose the "advanced" rule type you can make separate rules for pad and via connections:

enter image description here

If you're using a very old version of Altium that doesn't offer the "advanced" rule type, you can make two rules and use queries to apply one to pads and one to vias. If I recall correctly, there are "IsPad" and "IsVia" predicates available to specify which rule applies to which type of hole.

\$\endgroup\$
7
  • \$\begingroup\$ ok, so it sounds like the main concerns are manufacturability - not much wrt current capability, etc., unless one is pushing some limits - although then it would probably be easier to just add another via if possible. \$\endgroup\$
    – rothloup
    Mar 31, 2020 at 16:50
  • 1
    \$\begingroup\$ @rothloup, if you make the spoke width equal to the gap, you have "1 square" of copper no matter the dimensions, so the resistance of the relief pattern just depends on the copper thickness. If this is affecting the current capability, you may have to eliminate thermal reliefs altogether. \$\endgroup\$
    – The Photon
    Mar 31, 2020 at 17:21
  • \$\begingroup\$ Related article at EDN \$\endgroup\$
    – The Photon
    Mar 31, 2020 at 17:25
  • \$\begingroup\$ Thermal reliefs can already be eliminated for vias. Why would you need them on vias? Holes for THT components have enough space between them. Thermal reliefs are better for soldering. And an obligation if you want to solder them manually or have this possibility. It's very hard to solder a THT lead with an iron without thermal relief. \$\endgroup\$
    – Fredled
    Mar 31, 2020 at 21:38
  • \$\begingroup\$ @Fredled My CAD program doesn't seem to distinguish between vias and TH when forming connections to internal planes. So it's all or nothing I guess. \$\endgroup\$
    – rothloup
    Apr 3, 2020 at 11:59

Your Answer

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

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