I have seen this everywhere but cannot figure out why it would make sense to essentially compromise the quality of the ground connection. Is this done for visual reasons?
Here is an example:
\$\begingroup\$
\$\endgroup\$
1
-
\$\begingroup\$ There are times when using RF / Microwave devices that you do put a clamshell all the way around a component and include a ground connection all the way around. In those circumstances, you often have to solder the shell as a separate step probably by hand. This was for relatively low-volume high-cost times. \$\endgroup\$– TafTMay 24, 2019 at 7:39
Add a comment
|
5 Answers
\$\begingroup\$
\$\endgroup\$
6
This is to make soldering easier. Those 4 traces make it easier for the pad to heat up as the heat can only escape through those 4 traces. Soldering to a GND pad is difficult enough as it is, but if you had none of the spokes, you would essentially be trying to heat up the whole ground plane. It would be exceptionally difficult to heat it sufficiently to solder.
There may be some other reasons too, but this is the one that I know of!
As pointed out by @John Go-Soco in the comments, these are also reffered to as thermal reliefs
-
21\$\begingroup\$ They're sometimes referred to as thermal reliefs. altium.com/documentation/17.0/display/ADES/… \$\endgroup\$ May 22, 2019 at 7:49
-
1\$\begingroup\$ They're always called thermal reliefs.. You also do want to use full contact copper to make SMT connector more robust. That thermal relief pad will peel off fairly easily. \$\endgroup\$ May 22, 2019 at 9:27
-
1\$\begingroup\$ @Barleyman I've heard them referred to as thermal sinks in the past, but that's probably "unofficial". \$\endgroup\$ May 22, 2019 at 9:30
-
1\$\begingroup\$ @JohnGo-Soco Not to be confused with thermal pads, which are large pads found usually under the IC or for example on DPAK transistors. You perforate them with vias which will create a decent thermal connection to copper area on the other side of the PCB. \$\endgroup\$ May 22, 2019 at 9:41
-
1\$\begingroup\$ The gap in copper pour around the pad is called thermal relief. The connections cross the gap are called spokes. There are usually four spokes, but the number can vary. This is done with most copper planes and copper pours (not only for GND). \$\endgroup\$ May 22, 2019 at 21:34
\$\begingroup\$
\$\endgroup\$
5
It's worth mentioning that for reflow processing, thermal relief doesn't matter. The oven will take care of heating it. But for prototyping it becomes real PITA to (de)solder the pads.
That connector is an SMT connector. The thermal reliefs make the pads much weaker so it doesn't take that much vertical strain to peel them off the PCB. For mechanical strength it's better to leave the mounting pads as full contact, I don't think I've ever broken off an SMT connector that had solid copper on mounting pads.
-
2\$\begingroup\$ Very good point about the reflow process. I forgot to mention anything about mechanical strength so this makes a great additional answer +1 \$\endgroup\$– MCGMay 22, 2019 at 9:35
-
\$\begingroup\$ I have in fact laid out that PCB, it's for a microSD card. So when inserting the card there won't be any pulling forces only forces parallel to the PCB. I'm hand soldering, so that's a plus \$\endgroup\$– Wi_ZeusMay 22, 2019 at 11:56
-
1\$\begingroup\$ @Wi_Zeus A fair cop. Worst offender I've come across is a tiny U.FL coaxial connector. It really sticks to the connector so you need pliers to unplug it and the pads are quite small.. I once got a customer return with TH D-connectors twisted all out of shape, looking like someone took a hammer to the poor things. Being TH the connector wouldn't come off, thought.. \$\endgroup\$ May 22, 2019 at 12:14
-
2\$\begingroup\$ Thermal reliefs not mattering for reflow is mostly true, but not 100%. Consider a small two-pin SMD parts, such as 0402 resistor. If one pad is on a thinly connected pad and other is solidly connected to ground plane, there is some chance that solder on the thinly connected pad melts first and pulls the part up. This is called "tombstoning". \$\endgroup\$– jpaMay 23, 2019 at 17:43
-
\$\begingroup\$ @jpa Tombstoning happens with thermal reliefs as well as with just traces connected. And even with reliefs, it's considerably harder to solder the plane connected pad. I had assembly company that liked to make paste openings conical for chip components to combat tombstoning for what it's worth. \$\endgroup\$ May 24, 2019 at 11:29
\$\begingroup\$
\$\endgroup\$
They are commonly referred to as 'thermal relief', and as others state, they are to make soldering easier, as they impede thermal conduction to the rest of the ground plane. The thermal conductivity of metal is, like electrical conductivity, determined largely by the free electrons. So beware, this also impedes electrical conduction.
\$\begingroup\$
\$\endgroup\$
These gaps are for thermal isolation. If these weren't there you would be heating up the whole ground plane which could harm other nearby components because of the extended time needed to get to the required soldering temperature. This is less of a problem with industrial production but very much a concern in hobbyist soldering.
As for the quality of the ground connection: normally high frequency signals are captured by decoupling capacitors nearby the supply pins. This results in only a DC current over the ground plane which can easily pass through these smaller pathways.
\$\begingroup\$
\$\endgroup\$
3
'Star-connect' pads are basically a trade off between thermal conductance and structural strength. The usual case for a pad de-laminating is for an edge to peel up. The star structure holds all the edges down, it's actually stronger than some of those other pads in the picture.
As to why you want to limit thermal conductance, that's not just confined to assembly considerations. While heat may not be an issue in a lot of designs, it can certainly be a major consideration in others. Ground planes and other copper fills are often used to stink heat off your small surface mount parts. So thinking about how much a component sinks and where could be important to a design and you can't always have the physical spacing between components that you might otherwise want.
Why that particular board uses them. Well it seems a little odd... Those are the pads for the SD slots external casing. It's clearly a surface mount design, so you would expect a re-flow construction where heating the pads isn't a problem.
Perhaps the SD slot has plastic components that aren't spec'd for the oven temperatures and so had to be attached separately? Or if it was a DIY/Hobby kit then that would also make sense. Of course someone could have just ticked the 'star-connect' box when they routed the ground connections in their EDA software...
-
\$\begingroup\$ Thanks for the elaboration! I designed this particular PCB myself and honestly didn't pay much attention to details like these. It's a hobby project that will go through several revisions. I'll hand solder the components. The microSD connector does have plastic parts. \$\endgroup\$– Wi_ZeusMay 22, 2019 at 15:43
-
\$\begingroup\$ If the SD card slot becomes unreliable and has to be replaced, thermal-relief pads will make rework much easier if one takes care to remove all the solder before trying to remove the part. \$\endgroup\$– supercatMay 22, 2019 at 16:28
-
\$\begingroup\$ It's a good idea for prototypes and anything you're going to attach by hand. Those metal casings can be difficult enough to heat without having the entire ground plane sucking up the heat as well. You really don't lose that much strength, especially for a light force application like the SD card. \$\endgroup\$– heketeMay 23, 2019 at 3:05