0
\$\begingroup\$

I have a 4 layer design, Top, layer2, layer3, bottom. Now I want to place GND vias on a ground polygon. Layers Top and Bottom both are a complete ground plane (Polygon)

I was wondering; What is the most effective way to place this GND via and what are the differences?

I realise that on the first picture, the GND via is connected to the top layer polygon. And on the second picture it is both connected to the Bottom and Top layer polygon.

enter image description here

FYI, looking at the Eagle design the GND vias are not ''repoured'' as they are on Altium.

enter image description here

Again, I am nog experienced with Altium. Maybe there is a setting which lets me place these GND vias as they are on Eagle. (If that is a correct method)

\$\endgroup\$
  • \$\begingroup\$ I'm curious - do you have a reason for having ground on top and bottom ? Usually ground is placed as one of the inner layers. \$\endgroup\$ – efox29 May 11 '16 at 6:55
  • \$\begingroup\$ Are you talking about the thermals? The altium vias have thermal relief. The eagle vias seem to have no thermal relief. \$\endgroup\$ – mkeith May 11 '16 at 7:04
  • \$\begingroup\$ I am a intern trying to understand the design, and redesigning it as I migrate it from Eagle to Altium. \$\endgroup\$ – Jordakoes May 11 '16 at 7:11
  • \$\begingroup\$ @mkeith If I understand correctly, the vias in Eagle are ''Direct Connect'' and the vias in Altium I am placing are ''Relief Connect'' \$\endgroup\$ – Jordakoes May 11 '16 at 7:37
  • \$\begingroup\$ Right. Is that what you were most curious about? The fact that the Altium vias have voided copper areas around them? I think efox29 explained that well. \$\endgroup\$ – mkeith May 11 '16 at 7:42
4
\$\begingroup\$

You place a via and assign it to the ground net. That's it.

If you are lazy, like me sometimes, I sometimes place the via directly on the net I want the via to be - this can be another trace, polygon, even a pad (and then move it later) - and Altium will automatically assign the via's net to whatever net you placed the via on.

You should probably change your rules so that vias don't add thermal reliefs. You'd want direct connect (unless you plan on soldering things to it).

Create a rule similar to the image below, and that will make all your vias direct connect.

enter image description here

\$\endgroup\$
  • \$\begingroup\$ Thank you for taking time to answer my question, now what exactly is the difference between Relief connect and Direct connect? (Currently my rule are set to Relief connect.) \$\endgroup\$ – Jordakoes May 11 '16 at 7:08
  • \$\begingroup\$ Thermal reliefs are "special" way of connecting a via to a large copper body (like a plane or polygon pour). Copper is a good heat conductor, so it makes soldering very difficult because the pour or plane acts as a heatsink. If more information is required - this should be posted as a new question (if it hasnt already been answered already). \$\endgroup\$ – efox29 May 11 '16 at 7:15
  • \$\begingroup\$ I know that on another design there was a separate layer used as ground polygon. And on this layer the via connect style was relief connect. So now I am not sure what style to use. Although, I can always use one style. Then when it is incorrect, I can change to the other style without having to replace all the vias. So I quess I am just going to place all GND vias using the ''Direct Connect'' style. \$\endgroup\$ – Jordakoes May 11 '16 at 7:20
  • \$\begingroup\$ Most of the time, vias don't need thermal relief for electrical purposes. But through-hole pins do need thermal relief, otherwise they will be difficult to solder. The problem is that the soldering iron will be trying to heat the entire plane. The thermal relief makes a very noticeable difference in that case. Some SMT components have a large thermal pad in the middle of the component. The pad is part of the GND net. Normally the datasheet says to put lots of vias in the pad. Those vias are for heat conduction purposes, and should NOT have thermal relief. Those vias should be direct connect. \$\endgroup\$ – mkeith May 11 '16 at 7:51

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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