3
\$\begingroup\$

I have the upper layer of my board set up as GND copper plane.

However, when GND pads are connected to the GND plane, they are not completely connected to GND. Rather, a cross is formed on the pad. For example:

enter image description here

I wanted the whole pad connected to GND. How can I change that?

\$\endgroup\$
0

2 Answers 2

12
\$\begingroup\$

No Thermal Relief - Do you really want to do that?

Thermal reliefs are enabled by default for a reason. Large copper planes act like an excellent heatsink for the circuit board. This is both a blessing and a curse - pads connected to the plane can be more difficult to solder, desoldering is a bigger problem - in the worst case, a through-hole pad connected directly to a ground plane can be a repair/rework nightmare.

The problem is less serious for surface-mount pads, since reflow soldering usually heats the entire board evenly. But you may still encounter solderability problem, especially during the assembling and reworking of a prototype by hand.

There's a tradeoff between performance and solderability. If you don't have any special electrical or thermal requirements - such as better thermal conductivity for heat dissipation, a continuous ground plane or lower impedance for high-speed circuit, etc. - it's recommended to enable thermal reliefs.

Disable Thermal Reliefs Globally

To disable thermal relief for all copper pads in the entire ground pour, click the copper zone to highlight it on the screen, then press E to open the property dialog window.

In the property window, one can see the "Pad Connections" options:

  • Solid: disable thermal reliefs entirely
  • Thermal reliefs: enable thermal reliefs
  • Reliefs for PTH: only enable it for through-hole pads.

Copper Zone Properties

Disable Thermal Reliefs Locally

To disable thermal relief for a single copper pad, click the copper pad of a specific component, until only the copper pad zone is highlighted on the screen (but not the entire component, you may need to click the pads multiple times before that happens). Then press E to open the pad dialog window.

In the property window, one can see the "Connection to Copper Zone" options. The default setting is to follow the setting of the entire component, but it can be overridden too.

Pad Properties

\$\endgroup\$
3
  • \$\begingroup\$ The reason I want to have big GND pad connections, is beacuse when I asked this question: electronics.stackexchange.com/questions/674970/… user lindayin said that The trace width of the power and ground should be as wide as possible. I thought this should apply to pads as well. Is it wrong reasoning? I don't have too much of a pcb design experience. \$\endgroup\$ Aug 21, 2023 at 21:30
  • 1
    \$\begingroup\$ @user1584421 The sheet resistance of 1 oz copper is about 0.5 mOhm per square, and that thermal relief is four squares in parallel, so overall, the thermal relief forms approximately a 0.12 mOhm resistor (in other words, about 0.00012 ohms). If I had to guess, I'd say that's probably not going to be a problem for you. \$\endgroup\$ Aug 22, 2023 at 11:33
  • 1
    \$\begingroup\$ @CassieSwett: Another way of saying that would be to observe that a 100 mil trace that's 1cm long will have the same resistance as a 10 mil trace that's 1mm long. Narrow traces generally aren't a problem if they're short. \$\endgroup\$
    – supercat
    Aug 22, 2023 at 21:09
3
\$\begingroup\$

That is perfectly normal. It is called a "thermal break" - it provides some thermal isloation between the pad and the plane. Without that thermal break, you would have to heat a large area of the plane to get the solder on the component to stick to the copper plane.

\$\endgroup\$
4
  • 1
    \$\begingroup\$ If you’re going to reflow the board then dispensing with the thermal relief is less of a problem as the entire board will be heated to soldering temperature, but if you’re assembling by hand then an unrelieved pad will be very challenging to solder satisfactorily. \$\endgroup\$
    – Frog
    Aug 21, 2023 at 19:45
  • 1
    \$\begingroup\$ @Frog There's a tradeoff between electrical performance and solderability. For some applications, one may have a justified reason to manually override and disable thermal relief. For example, a coax connector requires a carefully-tuned ground plane cutout for a smooth transition. \$\endgroup\$ Aug 21, 2023 at 19:49
  • \$\begingroup\$ The reason I want to have big GND pad connections, is beacuse when I asked this question: electronics.stackexchange.com/questions/674970/… user lindayin said that The trace width of the power and ground should be as wide as possible. I thought this should apply to pads as well. Is it wrong reasoning? I don't have too much of a pcb design experience. \$\endgroup\$ Aug 21, 2023 at 21:31
  • 2
    \$\begingroup\$ There is a trade-off between optimum connections and easy solderability. With the thermal relief you effectively have four very short tracks connecting the pad to the ground plane which represents a minimal loss of connection with a considerable improvement in ease of soldering. Using thermal reliefs is very common. \$\endgroup\$ Aug 21, 2023 at 21:38

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.