I’m trying to put together a small board with Eagle-4.15…I’ve used the polygon fill to put ground planes over most of the board that’s not carrying some other signal, and I’d like to put vias from top to bottom in the ground plane to improve thermal conduction & reduce impedance. However, whenever I put in a via (or a hole), Eagle outputs Gerbers that have a border around the via, so it’s not connected to the rest of the ground plane. Also, pads that are supposed to be connected to the ground plane have empty rings around them, and are only connected by wires in a “+” pattern.
(These are screenshots from Eagle and ViewMate, respectively. Eagle doesn’t show the ring around the vias in the ground plane, but ViewMate does.)
How can I set up plated-through holes at random locations in the ground plane, and how can I get pads that are supposed to be connected to ground, connected all the way around?[/img]
Oops, following up to my own post…if you “Name” the vias the same as the ground signal, Eagle will connect them properly. So now I just have to figure out how to get the ground pads connected better…maybe by changing the default width of the signal…
Perfect, it works! I have to change the attribute in my libraries (not just on the board) but it’s not too hard.
Is there a (thermal-related?) reason I shouldn’t allow it to hook pins completely to the ground plane? On the amplifier, I know I’m supposed to do exactly that, but what about, e.g., the power jack. Complete connections should lower the resistance a little, but will the resulting structure be more likely to crack or fail?
spacewrench:
Is there a (thermal-related?) reason I shouldn’t allow it to hook pins completely to the ground plane?
I was just about to ask the same question. What is the purpose to the “+” arrangement. What is “thermal” about it? I have not re-activated “thermals” but I am considering it.
spacewrench:
Is there a (thermal-related?) reason I shouldn’t allow it to hook pins completely to the ground plane?
From the EAGLE manual (6.4 Multilayer Boards):
Pads are connected to power supply layers with what are known as thermal symbols, or are isolated with annulus symbols. Thermal symbols usually just have four thin bridges as a conductive connection to the through-plated hole. They are used because the high thermal conduction of a continuous copper plane would result in the pad being no longer solderable.
Pads are connected to power supply layers with what are known as thermal symbols, or are isolated with annulus symbols. Thermal symbols usually just have four thin bridges as a conductive connection to the through-plated hole. They are used because the high thermal conduction of a continuous copper plane would result in the pad being no longer solderable.
Yikes, that would be bad. Maybe I should switch back.
Well, “No longer solderable” is quite wrong indeed - I’ve worked on some 105µM-foil boards without thermals and with some pretty large planes, and I just had to crank up the temperature on my 80-watt Weller station a little bit.
If I put high-powered components in a design that I know will require extensive heatsinking, I always disable the thermals for that part.
Right, I’m having a similar problem to other people on this thread. I’m have a 2 layer board, with a ground plane on both sides. I want to connect the 2 ground planes together with vias.
However, when I add a via to the board and rename it to GND I don’t get any thermals… I really want thermals!!
Try selecting Change|Thermals|On from the left hand side, and clicking on the edge of your ground polygon. The thermal attribute is probably “off” on them.
The software I use has a thermal option for vias. It might be useful for high-reliability boards where all the holes need to be filled with solder, to ensure that the PTH doesn’t fail.
Yeah, “no longer solderable” is definitely en exaggeration. Maybe some automated soldering techniques (wave soldering?) have trouble with them, I don’t know, but if you’re hand-soldering it just makes things a little more difficult, since the ground plane sucks the heat away. In your case, of course, you want high thermal conductivity, so go for it.
When I’m hand soldering, I can definitely see the difference between a normal pad and one connected to a plane, even with the small cross pads, so, if it was connected directly to a plane it would make things even harder.
When I’m hand soldering, I can definitely see the difference between a normal pad and one connected to a plane, even with the small cross pads, so, if it was connected directly to a plane it would make things even harder.
Hmmm nice suggest. Simple you can solder it with plain but it has one side effect which is when atmosphere will bad, all signals will drop. For perfect procedure of wireless signals what brands you use ?
