|
When creating a ground plane in Eagle, Eagle automatically creates a thermal isolation for the pad. My first question is, does this isolation limit the current compared to a pad that is "completely" connected to the plane? My second question is, is there a way to make Eagle not automatically create a thermal via? I know one work-around: I can connect the pad with a thick wire then make that same wire on the ground plane. Unfortunately this is hard to do and can introduce errors. |
|||||||
|
|
The Eagle term for this is "thermals". The basic idea is to limit the connection to the plane or polygon fill so that it is easier to solder. I believe that this is the default behavior for Eagle, although the default settings do not make it "easy" to solder. These thermal via patterns will increase the resistance through your polygon fill, but not by a whole lot. Often you will have four connections to the plane, as well as your original wire connection (assuming you make sure everything connects manually before you begin to use polygon fills). The easy way to prevent Eagle from making thermal vias is to disable them in the fill polygon. You can do this by selecting the "no thermals" option when you are creating the polygon (see image below), or to modify the properties of an existing polygon fill and unchecking the box labeled "Thermals".
|
|||
|
|
|
The common name is "thermal relief". No, it doesn't limit the current. For changes in current the resistance must be at least, say, 1 % of the other resistance. My rule-of-thumb: a 1 mm trace of 35 µ, 1 m long has a resistance of 0.5 Ω. The length of the spokes is determined by the backoff. My design rules have a standard 0.2 mm for that, and I use a 0.35 mm width. Then the resistance of one spoke is 0.5 Ω x 0.2 (mm/mm) x 0.35 (mm/m) = 35 µΩ. Then 4 spokes are 9 µΩ. You can immediately see that this is negligible. a 5 A current will cause a 44 µV drop, and a 55 µW dissipation per spoke. |
|||
|
|
