The quote below is from the Eagle help file. I typically use polygons for ground plane pours and I'm pretty sure I've increased the isolate value to be larger than the clearances in the design rules and have not had problems. But evidently I don't know "exactly what I am doing" because I'm not quite visualizing what problems might occur, and whether they are detectable before having the boards manufactured. Can anyone shed any further light on this?
Isolate
Distance between polygon areas and other signals or objects in the Dimension layer (default: 0). If a particular polygon is given an Isolate value that exceeds that from the design rules and net classes, the larger value will be taken. See also Design Rules under Distance and Supply, respectively. Note that if you give a polygon an Isolate value that exceeds that from the design rules and net classes, small gaps may result between the calculated polygon and objects belonging to the same signal as the polygon itself, which may lead to problems during manufacturing! It is therefore recommended to leave this parameter at 0, unless you know exactly what you are doing!
Leave isolate=0 and stop worrying? Set it to a stupidly large value and see what happens?
I suspect its there for when you have high voltage fill you want to keep away from other signals, or if you want to reduce parasitic capacitance of a ground plane for RF layout.
MarkT:
Leave isolate=0 and stop worrying? Set it to a stupidly large value and see what happens?
Ah yes, the stupidly large value, great idea, now why didn't I think of that! XD
I tried a 100 mil isolate. Not surprisingly, what happens is the ground plane falls apart into multiple polygons, breaking ground connections in several places. Airwires appear that make this obvious. But the risk may be that with a not-so-stupid-but-still-too-large value, the same thing happens and the airwires are so small they don't get noticed. This is one of my pet peeves with Eagle, very short airwires can be hard to see. But there's no excuse for not knowing they're there, because the ratsnest command indicates the number of airwires on the status bar.
Still confused on the language in the help item, "small gaps may result ... which may lead to problems during manufacturing" makes it sound to me like the gaps are undetectable or nearly so. But as long as an airwire gets created, even if it's hard to see, ratsnest lets us know it's there.
When I make boards, I usually set the isolate value to one of two. If it is a densly packed board with limited space I use 12mil, whereas for large boards with lots of space I use 24mil. I have never had a problem with either.
If there is no soldermask, it is best to use a large isolate - say 40mil to reduce the risk of solder bridges.
For high voltage (I did a board with a 240V relay), I used two polygons on the same layer, one around the relay, one for the rest of the board. I set the Isolate next to the relay to 150mil to keep the ground away from the HV for safety reasons. (For even higher voltage - 27kV flyback transformer anyone? I would go even larger, say 500mil, or even remove the ground plane in that area all together to make sure there is no arcing).
Ahh, I mean to mention, you might find this useful (right click, save as... make sure the extension is set to .ulp. If it tries to save it as a .txt file, just save it and change the extension once it has downloaded) http://ftp.bricsworld.com/EAGLE-FILES/ulp/zoom-unrouted.ulp
If you save it to the desktop or wherever (you can copy it into the 'ulp' folder in the eagle program folder, that makes it easier to use).
Then, when you think you are finished, click the ULP button and navigate to the folder you saved the file and select that. If you saved it in the eagle directory I mentioned, you can just type "run zoom-unrouted" (without the quote marks) in the bar at the top of the pcb editor and press enter.
Basically it zooms right in on the first air wire it finds, then once you have corrected it, you run the ulp again to find the next and so on until it says 'finished' at the bottom of the screen at which point there are no more.
If it zooms right in to a spot on the power or ground plane but you can't see an air wire there, it means that bit of the plane is isolated from the rest (there is a tiny air wire, but you can't make it out).