Ground Pour |
Next I am going to edit/change some of the properties of this ground pour. All of these properties can be changed with mouse clicks, but showing that in a sequence of images is time consuming. So I am just going to give the equivalent keyboard commands and hope that you can figure out the mouse versions if that is what you prefer to use.
First, I am going to change the distance that the ground pour keeps from everything else. Enter into the command line
change isolate 24
or just “ch iso 24″ and then click on the edge of the ground pour. The result looks like this
so that all the gaps are narrower. At the beginning of this tutorial, I typed “ch iso 40″ so that I have reduced the ISOLATE parameter form 40mils to 24mils. That is what sets the distance between the ground pour and everything that is not grounded.
Second, I am going to change where the ground pour appears. Enter into the command line
change orphan on
or just “ch orph on”, click on the edge of the ground pour, and you will see this:
This caused islands of ground pour to appear between C2 and C3 and between R3 and R5. These are called orphans by Eagle and they are not connected to the original ground pour. You will see that in my layouts I leave the ORPHANS parameter off and that is the value that I set at the beginning of the tutorial.
If you type
change width 10
and click on the edge of the polygon next then you are changing the 40mil width that I set at the beginning of the tutorial to only 10mils. This changes the image above to
so that the pour appears in narrower gaps between traces.
One more parameter change: enter “change thermals on” and click an edge of the polygon. This time you may not notice a difference at first. Here is an enlargement of the lower left-hand corner:
What you see is that the pads are partially isolated from the rest of the ground pour. The thick connections are the 40mil traces that were there before putting in the ground pour. The thinner connections are 10mil traces (because that is the WIDTH parameter we chose above) created by the polygon. These are called THERMALS because they prevent the ground pour from acting like a heat sink when one is soldering connections to them.
I am almost finished writing this tutoral. I need to make a few closing remarks comparing the DELETE and RIP commands, the POLYGON_RATSNEST paramer, and how to make sure that VIAS have thermals just like PADS. I will probably do this sometime over the weekend.
Kirby said:
great tutorial… exactly what I was looking for
Posted 14.11.2007 at 9:44 am
gaussmarkov said:
Excellent.
There is more. I have the images already. I just have to find the time. 
Posted 14.11.2007 at 10:00 am
Auke Haarsma said:
Keep m coming! Great tutorial!
Posted 08.02.2008 at 5:16 am
the said:
ch lay bot does not work…
got a tip?
greets
Posted 01.03.2008 at 6:52 am
gaussmarkov said:
the,
your message is too cryptic to offer a tip. there are times when “change layer bottom” does not prevent the route tool from reverting to the top layer when you are starting a new trace from an existing trace that is in the top layer. that’s all that comes to mind and that’s just eagle. you have to take your mouse up to the route tool bar and click on the layer you want.
good luck, paul
Posted 03.03.2008 at 8:59 am
Roman said:
Thanks for the tutorial AND the libraries, this is extremely useful for noobs like me. Your detailed description of the ground pour is the best I’ve seen on the Net, thanks for taking time to do this!
Posted 24.03.2008 at 6:20 am
gaussmarkov said:
hey Roman,
it’s a pleasure to get appreciative feedback like yours!
cheers, paul
Posted 24.03.2008 at 8:44 pm
Allan said:
Loving these tutorials, got my first pcbs started with your help. Thanks.
I’m having trouble getting my top and bottom layer pours to ‘work together’ they are wiping out traces in each ones level. Like this:
http://i26.photobucket.com/albums/c143/ringworm_1974/Picture1.png
Any tips? is there a way to make a board with just a single layer, this would seem to make sense for small stompbox projects, or am i misunderstanding something fundamental about pcb design?
Posted 23.12.2008 at 4:29 am
Allan said:
I got it figured out! I was clicking on the pour rather than the traces to change the layer.
Posted 30.01.2009 at 7:02 am
Rufio said:
Great tutorail gauss, thanks for the librarys. I made my first pcb, i don’t know if its going to work, but looks ok.
Are you going to continue this tuto? I had trouble withe the tool “autorute”, didn’t like the way the ground line came out.
How do you make de ground line stays around the pcb?
And finally how do i export my pcb to another program, like photoshop, to print it, with other pcbs?
Posted 19.06.2009 at 5:20 pm
Anonymous said:
good tuto
Posted 12.09.2009 at 3:29 pm
Anonymous said:
nice ..
Posted 12.09.2009 at 3:29 pm
RNFR said:
i’ve found that ch wid 1 makes your ground pour edged much cleaner and nicer looking. give it a shot!
and thanks GM, i still refer here often!
Posted 07.11.2009 at 1:57 pm
Parker said:
Great tutorial, but what do those six commands actually do? Becasue now eagle thinks my board is actually 3.7 metres across and I cant seem to change it back…
Posted 08.03.2010 at 2:26 pm
Parker said:
Ah sorry my mistake I was assuming ‘mil’ was short for ‘millimetres’ which apparently it isnt? Must be a yank thing…
Again this is a fantastic tutorial – cheers
Posted 09.03.2010 at 11:40 am
Hawg said:
gm-
I also got the error when I entered the ch lay bot command, because I was still working from the new->schematic from the last tutorial.
If anyone else gets the error, it might be because you are working on a schematic instead of a board. Right click your project and go new ->board.
Posted 08.06.2010 at 12:48 pm
paijo said:
this is what i need…thanks
Posted 11.06.2010 at 1:55 am