1
\$\begingroup\$

I am using a polygon pour to connect to the pads in the image shown.

What I do not like about it is that you only get those (maximum of) 4 little traces of copper that actually touch the pad - is there a way to have pours that completely cover the pad in copper, like in the second image?

I have tried using Fills and Solid regions on the top layer, but Altium does not seem to like that, even when I have the nets correct - am I doing something wrong?

enter image description here

enter image description here

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Those four little traces are there for a reason! They're called thermal reliefs, and they make soldering much less of a pain. \$\endgroup\$
    – Hearth
    Jun 30, 2021 at 4:20

2 Answers 2

3
\$\begingroup\$

You can eliminate the thermal reliefs but it's not a good idea for pads (it's okay for vias that don't have anything soldered to them).

The reason is that the polygon (or plane) will suck too much heat from the pad and the soldering may not be good.

Anyway, here is the rule you can adjust (it's under 'Plane' in the Design Rules, so maybe not obvious):

enter image description here

On this simple PCB I have only two rules, the default one for pads as shown and another that applies only to vias where the connect style is specified as 'Direct Connect'. It should probably have a more descriptive rule name than the 'PolygonConnect_1' default.

\$\endgroup\$
1
  • \$\begingroup\$ OP - Thermal reliefs are recommended but you could also talk to your assembly house - I've had production boards without thermal reliefs on some components and they went fine because the assembly house told me had processes in place for things like that. \$\endgroup\$
    – efox29
    Jun 30, 2021 at 5:53
1
\$\begingroup\$

You can use fills and solids, but you need to change the net lable to match whatever traces or pads the fill is running over or connected to.

But this is not a good way to approach your particular problem, those pads need thermal relief for soldering (which most PCBs have components soldered to them one way or another). The problem is without the reduction in copper around the pad and a large fill or power plane, The heat quickly bleeds out of the pin of the component and into the plane which lowers the temperature and makes it very difficult if not impossible to solder.

So leave the thermal reliefs in the design, they only amount to a few milliohms of resistance anyway.

\$\endgroup\$

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.