5
\$\begingroup\$

I have prepared the following PCB layout

enter image description here

I am a hobbyist and when I look at other - professional - boards, mine looks a little strange when considering the empty spaces to the right, and to a lesser extent to the bottom. But Eagle refuses to fill these spaces with GND conductor. I suppose there must be a setting in Eagle that controls fill polygon separation, but is it worth bothering at all?

I have learned (or at least I think I have) that in layouting for analog circuits, especially in the high frequency domain it is very important to have the ground area as close to the signal lines as possible in order to reduce capacitive coupling to environment noise. Preferably a separate dedicated ground plane.

But in my case it is just a pure digital circuit, and it's only up to 20 Mhz clock speed. The circuit works perfectly on my desk, but I have no idea as far as its EMC properties are concerned.

How would I go about the empty spaces? Should I try and separate the other lines until GND can fill the spaces, even if it means enlarging the board? Or should I leave them as they are?

\$\endgroup\$
  • \$\begingroup\$ Do you have ground on another layer too? \$\endgroup\$ – pipe Jun 2 '18 at 16:28
  • \$\begingroup\$ @pipe: nope. With only one layer it's easier for me to etch quick prototypes at home with the help of my 3d printer (scratches negative out of coating; use FlatCam for generating gcode; aka isolation routing, sort of) \$\endgroup\$ – oliver Jun 2 '18 at 16:31
  • 1
    \$\begingroup\$ Ok, because then you need to start looking at how your ground pins are connected, and the ground island you are looking for will make this even harder to see. For example, the ground pin on your 4-pin connector to the right has a loooong way to go to the ground on the 6-pin connector also to the right. \$\endgroup\$ – pipe Jun 2 '18 at 16:36
  • 1
    \$\begingroup\$ Sorry this is a bit off topic, but why do these traces not just go straight down? i.imgur.com/2Kswzxk.png \$\endgroup\$ – 12Me21 Jun 3 '18 at 3:58
  • \$\begingroup\$ @12Me21: you're absolutely right. Originally there was a wire bridge in this area, and the trances went around it. Thanks for pointing out. \$\endgroup\$ – oliver Jun 3 '18 at 6:08
4
\$\begingroup\$

Type "Change", then select "Orphans", then "on". If you click now on your polygon pour, it will fill the gaps. Be aware, they are not connected to ground, just blank copper. Another option is to reduce the "Isolate" value; that will allow your pour to move closer to the traces/holes. Check your manufacturing limits if you try that. Most boards these days are two sided, so it's usually possible just to put a via through. (There's very little price difference for hobbyists to go two sided over single sided, worth thinking about.)

Based on your layout, there is a few things you could do without changing the board size. If you move the component (resistor?) in the middle above the IC left and down a little, you could move the trace which goes underneath it down a little as well. That way, the GND pour might be able to fill in sufficiently.

\$\endgroup\$
  • \$\begingroup\$ Thanks, very helpful trick. Do you think that it's problem, if there a are orphan regions on a board or is this quite common? \$\endgroup\$ – oliver Jun 2 '18 at 16:26
  • 2
    \$\begingroup\$ @oliver Yes, it can be a problem as they can act like little antennas. Also, depending on the manufacturer, infill copper is sometimes preferred and sometimes not. On your board, I wouldn't be too concerned about it - the gap's not big either, just exaggerated by the image. \$\endgroup\$ – awjlogan Jun 2 '18 at 16:29
4
\$\begingroup\$

Should I try and separate the other lines until GND can fill the spaces, even if it means enlarging the board?

Alternatively, you should consider reducing the spacing between traces, which will leave more space elsewhere for the pour.

For example, the three longish traces across the bottom could run right next to each other, and they could also take more direct routes to the pins on the left.

\$\endgroup\$
  • \$\begingroup\$ That's what worried me as well. But it's the default separation Eagle offers me. Of course I can override it easily with Alt+<drag> during positioning, but I hesitated to do so because I thought there was good reason for choosing these values as default (particularly for amateurs like me). \$\endgroup\$ – oliver Jun 2 '18 at 16:42
  • 3
    \$\begingroup\$ Use a finer grid for routing in the first place. \$\endgroup\$ – Dave Tweed Jun 2 '18 at 16:45

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.