Supply Layers in Eagle

Community PCB Design
1

Hello all,

This is my first time making a board in Eagle. I have 4 layers in this design and the two inner layers are Vdd and GND. The through-hole components have automatically been connected to the supply layers but I’m not sure how to connect surface mount components to the supply layers. Should I be using Vias? From eagle docs: “The layers Pads and Vias have nothing to do with the Supply layer”.

As a second question; how can I draw an “Isolating Wire” around the edges of the board? What layer should this be? Eagle docs:

“To keep the board edges free of copper draw an isolating WIRE near the border. This avoids possible short circuits between adjacent (Supply) layers.”

And finally, does anyone have any general advice when using supply layers.

Thanks,

Anthony

2

antdengineer:
This is my first time making a board in Eagle. I have 4 layers in this design and the two inner layers are Vdd and GND.

A four layer PCB is quite a bit more work and cost than

two layers. Why do you need four?

antdengineer:
The through-hole components have automatically been connected to the supply layers but I’m not sure how to connect surface mount components to the supply layers. Should I be using Vias?

Yes. If you turn off all layers except "Dimension" and

“Unrouted” (19 and 20) you should see air wires from

every SMD/SMT pad that has not been routed.

Use the “SHOW” tool (or type “SHOW ”) to

highlight your power and ground nets, one a time.

Manually route these and use vias to ‘staple’ the outer

layers to the inner planes.

A completed PCB will have zero (I mean none, not any,
not even little specs) on the Unrouted layer.

Turn off the grid and all other layers to check this very

closely. Just one of these will bring you a “green coaster”

instead of a PCB later!

antdengineer:
how can I draw an “Isolating Wire” around the edges of the board? What layer should this be?

This is probably something lost in translation...

I think it means that you should draw a poly around

your inner layers, and adjust the size to be inside the

physical PCB border. When fabbed the inner layers

will then have a non-metal perimeter clearance to

stop the layers form shorting together.

antdengineer:
And finally, does anyone have any general advice when using supply layers.

Avoid them if possible for low cost, easy to do

projects. (Unless you have no choice…)

3

Thanks for your informative response!

I am now routing traces to the ground/power layers.

4

I have routed my entire board but im still confused about the “Isolating Wire” around the edges of the board. What layer would this be?

5

Just make sure the DRC Rule “Copper/Dimension” under the tab “Distance” is 8mil

or higher. (alternatively use Sparkfun’s DRC Rules)

(the “Isolating Wire” is used so that if you were to shear a panel of PCB’s apart,

the copper on the inner layers won’t short together with tiny flakes of metal along

the edge of your boards)

6

Ok, that makes sense. I do have that rule set.

7

Has anyone had any experience with generating gerber files for a 4 layer board (particularly one with the two internal layers being supply layers) ? I’m thinking i could just modify the sparkfun cam file but i dont want to do this wrong since supply layers work in a special way in eagle.

8

I realized that the isolating wires for a given signal layer need to be drawn using that same layer. This will lead to a lack of copper in the shape of the trace because drawing using an inverted layer actually means your specifying where NOT to put copper. So basically there will be a thin band of no copper around the entire board on both signal layers. Two perimeters need to be drawn; one on each signal layer.

As far as CAM jobs go I think there just needs to be two additional gerber files that only include one layer each (PWR or GND) and no vias or anything else. Is this true? I’m still not sure if I need to do something special because of the inversion.

9

antdengineer:
As far as CAM jobs go I think there just needs to be two additional gerber files that only include one layer each (PWR or GND) and no vias or anything else. Is this true? I’m still not sure if I need to do something special because of the inversion.

I’ve done a 4 layer board. Just add your 2 plane layers to the CAM job. An EAGLE plane layer starts with “$” (i.e. $GND). You don’t need the “via” or “pad” layers for the plane layers.

-Dave Pollum