HOW-TO: Polygons and ground fills for PCBs in Eagle
In Eagle polygons are used to make big copper areas on a PCB that aren’t necessarily traces. We use them all the time to fill blank space on a PCB with copper connected to ground. Less frequently we use them to make large power traces such as with the ATX Breakout Board. Here’s some notes on how to use and customize polygons in Cadsoft Eagle.
How to use
Open Eagle and start a new schematic and PCB. Go to the board so we can lay down a polygon.
- Click ‘polygon’ icon
located in the toolbar - In the top menu bar make sure the top (red) or bottom (blue) copper layer is selected
Route the polygon in the shape you want it. Make sure to close it at the starting point or you’ll have problems generating gerbers later.
A polygon with a dashed line will appear (picture 3).
Click the ‘Ratsnest’ icon 
, and the polygon will fill with a solid copper area.
This will now be a solid copper area on your final PCB. Next we’ll look at a few ways to customize it.
Polygon Name
Sometimes it’s useful to make the polygon part of an existing trace or electrical net. For example if you wanted to beef up a power trace.
To connect the polygon to the ‘net’ you want, right click on it’s edge, and select ‘Name’. Here make sure ‘This Polygon’ is selected, and type in the net name you want it to connect to. Hit ‘Ok’.
Polygon properties
Right click on the edge of a polygon and select properties. This opens the ”Polygon properties” menu. From here you can customize the polygon.
Width
This is the width of the polygon’s perimeter when you draw it on the board. It also affects some properties below.
Pour
Here you can select between two versions of fill for inside the polygon, solid or hatched.
Hatched line widths are adjusted in the ”width” property. Line spacing is adjusted in the ”Mesh Distances” property. We only use the solid fill option in our projects.
Isolate
This is the clearance between the polygon and neighboring objects, such as other traces, pins, and other polygons.
Don’t torture your board house here. Low isolation values lead to PCBs with electrical faults from under-etching. Leave as much room as you can.
Ranks
Rank determines if one polygons if above or below an overlapping polygon.
Assigning a lower rank to one polygon will make that polygon dominate the other as seen in the pic above. When using a ground fill over the entire board it is important for it to have the highest rank so other polygons can be drawn.
Thermals
With thermals on, a pin will connect to the polygon through small traces extending from the pin center in 4 directions. Thermals make soldering easier, the part heats faster because the heat is not dissipated as quickly.
Disable thermals will make a solid pour trough the pin/pad. We usually use thermals. We only turn it off on high power traces that require more conductivity between the pad and the polygon.
Uses
Ground planes
Ground planes fill-up the empty spaces of a PCB with copper connected to ground. The ground plane connects all the ground pins on a PCB automatically, which usually makes routing easier. It can also reduce electrical noise on the board.
Filling the board with a ground plane is the first thing we do when designing a PCB.
- Draw a polygon
- Give it the same name as the ground connections on your schematic, usually ”GND”
- Click the ratnest button to refresh the ratnest after adding parts or traces
Any parts placed in the ground plane with pins names GND will automatically connect.
Power planes
Power planes are no different than ground planes, they just carry a power supply instead of ground. We use these for fat power traces where the board will carry a lot of current.
Power distribution for multiple voltage powered chip
Multiple supply polygons, good for power distribution especially on CPLD and FPGA chips.
Although a normal traces can be used here, concentric C shaped polygons provide both a power supply access, and give you more freedom with it’s shape.
This entry was posted in Eagle and tagged Eagle Polygons.
Comments
Is there really any difference in the number of shorts between two regular traces spaced at 8mils compared to a trace next to a ground fill with 8 mils distance? I’ve read it before in other texts that you should have like 14 or 16 mils isolation for ground fills even if the rest of the board is routed 7/7 or 8/8.
To me it seems a bit like an urban legend. Much like the famed “acid-traps” that apparently occurs when tracks connect/bend at 90 degrees or less angles (that would be Acute angles if I remember my math and English classes correctly).
I’m going to guess: Could it be that it’s not shorts but signal issues instead? Perhaps placing signals very close to ground will result in some stray capacitance that affects the signal shape, so 14 or 16 mils might reduce the capacitance by 1.75 to 2 times. But I don’t know how significant such tiny capacitances might be.
I have read that ground places under SMD chips can seriously create unexpected and undesired capacitance … to the point that some op-amp data sheets recommend defeating the ground plane under the SMD pads for critical or sensitive input pins. I’m not sure how much a parallel trace would have this effect as compared to parallel plates like an SMD pad over a ground plane.
What are HATCHED polygons for?
Hatched polygons are often found on boards with capacitive touch buttons. The hatched pattern creates less capacitance due to smaller area.
Thanks!
I’ve seen old boards that was wave-soldered (basically dipped into molten tin) that had its ground fills becoming all bubbly and wrinkled. Possibly from gasses released from the board getting trapped under the large copper area. A hatched fill would reduce this.
Probably this is not an issue with modern manufacturing techniques using FR4 laminate and reflow soldering.
And most laser printers produce a better result when doing printing a hatched area compared to a completely filled area when doing homebrew PCBs.
The amount of copper should be balanced between the board layers to reduce warping. Perhaps not a big issue with 5×5 cm boards or hand soldered homebrew but it is for larger boards and production panels.
The term “FR4″ can vary quite a lot between different manufacturers. We had a PCB supplier that used different manufacturers depending on volume and time, ie prototypes and mass production. The prototype boards were quite stiff, which was good for this 300×200 mm 4 layers board. The boards for mass production were much softer and tended to sag about 5 mm, even at room temperature, with all the components soldered to it.
Just a guess from my side, but was it not more popular with hatched polygons in the 1990s? Almost like it was a new feature in the ECAD software that he designers wanted to show of with.
Try to keep all polygons as intact as possible instead of just stitching with a single via. Do a rough layout and then move traces and vias, repour and try to get connections between polygons of the same net. Sometimes it is also worth the penalty of added vias to change the routing layer for a few segments just to keep the polygons more intact.
Look at the top row of components on the featured layout. The second pair of 0603s has a via that breaks the surrounding polygon. Move that via up a bit and perhaps also the via between the 0603s and then repour. The continue to do that for the rest of the board. Long and narrow copper areas that are not connected in both ends can also come loose and cause problems.
Through hole pads can also be trimmed to be more rectangular and sometimes with the holes off center, just to increase the spacing between the pads. Then the polygon might fit in between. With 10 mils trace and space you can have pads with up to 70 mils in diameter. Make sure that the copper around the drilled hole (annular ring) is within your manufacturers capabilities.
ANOTHER Eagle article ?
Come on, this thing is just a teaser for the commercial version and has lots of limitations. It’s free so you’ll invest the time in learning it and won’t want to bother with something else when you hit the limits.
There are other good packages around, KiCad especially. How about some articles on that ?
We use Eagle, so unfortunately we can’t write about KiCad ourselves.. This tutorial was made to help people learning Eagle….W’ll look for some KiCad articles online, and make posts about them, from time to time, but DangerousPrototypes only uses Eagle at this time, limited as it is… If and when we switch, we’ll surely share any insights we learn along the way.
Unfortunately right now we don;t have the time to switch to another ECAD, as that would probably involve porting all our projects, and libraries to it, and we just don’t have the time for such a massive undertaking…
Yes, I can understand that you wouldn’t want to switch – that confirms my point !
But thank you for offering to point out the alternatives, I’m sure that’s worthwhile.
I purchased a full, 3-seat license for Eagle and have designed several commercial products with it. Also, I know many professionals who use Eagle, some who pay and some who live with the limitations. Eagle is a very viable CAD program – it isn’t perfect, but there isn’t any out there that are perfect.
I’ve been using different CAD programs starting with Protel 99, P-Cad2008. I like Eagle mostly because it saves me a lot of time with nice parts library organization which I didn’t or still don’t like in other CAD. Most projects I do in Eagle also some BGA routing etc. I noticed that all CAD programs are actually the same in base for me. I just got used to Eagle and it is easier for me to use. Sometimes I miss some features that for an eg. Altium Designer has but… everything can be done with Eagle. Matter of taste! :)
I put on my chip a keep out “square” on the layer “tKeepOut” as there are exposed testing points there. I want my ground pour to go around this, is this the right way to accomplish this, or are there better alternatives? How can I check it will work, is generating a gerber the best/only way?
If your ground pour is on the Bottom layer, then copy your tKeepOut square and change its later to bRestrict. If your ground pour is on the Top later, then use tRestrict. The keepout deals with physical placement, while restrict controls copper generation and is useful for both traces and pours.
Thank you.
How can i increase the distance between the tracks and mask determined by the polygon ?
Hi iulian,
You can change the “Isolate” value. see Polygon properties picture above, to vary the isolation distance between mask and traces.
thanks for the tip … but i found out want i wanted to know : i managed to enlarge the isolation gap from Drc/clearance/wire ; i changed the “wire” value and that did the trick . Thank you for your help anyway !
No problem, that DRC trick will do too.
1. When polygon is created in eagle6.4.0 lite and 6.2.0 lite is created, it calculates correctly. Any layer.
2. When the same polygon is renamed into a some wire name from schematic, it does not calculate anymore at all. Any layer.
3. There is some 12mils limitation somewhere in the programe regarding width of polygone wires that cold not be found… Any layer.
How about that?
Thank You