Hi,
What is the difference between a solid ground/power plane and one that would come with a specific pattern (like a tiling pattern for example)?
I’m used to design PCBs with solid ground/power planes. I just came across a tiled ground plane and I’m not sure what it’s about.
Thanks!
I always use a solid groundplane. The “mesh” type was an old-fashioned method, and sometimes was used to help balance the amount of copper on different layers (to reduce warping of the board).
These days with high-speed circuits you want the ground plane to be as low impedance as possible, and that means a solid plane, not mesh. A solid groundplane is also much more effective as a heatsink for SMD components that rely on it.
It’s also a good idea (for EMC / high-speed reasons) to solder the ground pins of components directly to the groundplane if possible, rather than use “thermal reliefs”. This isn’t possible with hand soldering, but works with reflow, since the entire board is heated. I must admit I often don’t follow this advice myself though… Anything that you hand solder (eg though-hole components) should still have thermal reliefs.
Hi MichaelN,
Thanks for the detailed answer. I’ve also heard that ancient PCB CAD software used to generate mesh type ground planes to limit the amount of data sent to the manufacturing tools.
Do you see any specific recommendations regarding the ground plane, and more generally regarding PCB design, when designing devices that will be used in noisy area?
The device I am working on will be used in an high voltage environment (500kV). It will be enclosed in a metallic box, and will only be electrically conected to 60V signals. Any recommendations you may have?
Thanks!
MichaelN:
I always use a solid groundplane. The “mesh” type was an old-fashioned method, and sometimes was used to help balance the amount of copper on different layers (to reduce warping of the board).These days with high-speed circuits you want the ground plane to be as low impedance as possible, and that means a solid plane, not mesh. A solid groundplane is also much more effective as a heatsink for SMD components that rely on it.
It’s also a good idea (for EMC / high-speed reasons) to solder the ground pins of components directly to the groundplane if possible, rather than use “thermal reliefs”. This isn’t possible with hand soldering, but works with reflow, since the entire board is heated. I must admit I often don’t follow this advice myself though… Anything that you hand solder (eg though-hole components) should still have thermal reliefs.
For EMC reasons, it is actually sometimes cheaper & easier to go to a greater number of layers on the PCB, since that allows proper dedicated ground / power planes, which makes EMC compliance easier. Trying to fix an EMC problem later can be very time consuming & expensive.
Regarding analog / digital / split ground planes, these days it is normally not recommended. You are normally better to have a single ground plane, and segregate the board into analog and digital “zones”. In some cases, split ground planes are used, but you must be VERY carefull to take care about ground return paths. See my post here:
viewtopic.php?t=17715&highlight=
500KV is certainly high voltage! You’ll need to make sure all inputs and outputs are well filtered & protected. Also, at that voltage, the housing of the device is very important - such high voltages can arc through any openings in the metal (eg for switches, indicators etc).
Google PCB design for EMC and you will get a lot of contradictory advice. The reason is what works well at low frequencies often won’t work for high frequencies, and vice versa.
So without knowing the application it is difficult to comment. But here are some pointers for general low frequency design. These have helped me during the dreaded EMC compliance testing…
What works well for emissions will work well for immunity. (I’m assuming immunity will be your main problem with 500KV around it)
Keep current loops as small as possible. The area the current path encloses is the current loop, and the bigger it is the worse it is for EMC. If you are relying on the ground plane to take your signal back to the source then make sure your signal line sits over the ground plane (Loop = length of your trace x thickness of the laminate).
Have as much copper as practical, but don’t have floating copper. All planes must be grounded (or at potential).
Keep noisy tracks away from clean ones and don’t run them in parallel to each other.
Don’t be afraid of using multiple via’s. High frequencies and ESD often find their source by traveling over the surface of conductors. Multiple via’s give more surface area.
Caps caps and more caps. Don’t get stingy on a hand-full of passives.
ESD kills. Like Michael says - protect your inputs. You may replace the whole unit in the field, but blowing up semi’s during development sucks!
A box ain’t an EMC box unless it is truly 360 degrees conductive. O-Rings will give the whole game away. There are lots of cool conductive strips and seals out there. Even conductive bags. Once I used a clear conductive ink on a membrane keypad to complete a shield!
I could go on and on but I’m getting depressed. It’s all black magic anyway! :?
I agree with the comments by evarobotics.
I found Keith Armstrong’s advice on the following site very valuable on these types of topics. You have to register to see it, but they never send spam…
Keith Armstrong is ‘Da Man’!
One day I’ll get to go to one of his courses… Training budget? I have heard talk of these strange and frightening concepts from the new world!