Supply Layer

Community PCB Design
1

Hi,

I’ve been trying to get a grip on how EaglePCB handles inner layer ground planes. It appears that they have something called a supply layer to do this. From what I understand, given that your ground net is called “GND”:-

  1. Create a new layer. (This usually goes to 103, I can’t get any lower.)

  2. Name the layer “$GND”.

  3. This will automatically display as “GND”.

  4. This will now automatically serve as an inner layer.

  5. Anything you draw on this layer actually removes copper instead of adding it.

In other words, you don’t have to draw anything on this layer, except perhaps a border to keep the ground plane clear of the edges.

Well I’ve done all this but for some reason, the GERBER files that the CAM processor generates for this layer is empty. Am I missing something here? Any help will be greatly appreciated.

Regards,

Daniel

2

I don’t know the ‘official’ way to do it, but why not add a polygon named ‘gnd’ to the layer as you would to the top or bottom layers. It works the same way you describe, any traces you add inside the polygon “remove” copper from it.

3

Daniel Wee:

  1. Create a new layer. (This usually goes to 103, I can’t get any lower.)

  2. Name the layer “$GND”.

  3. This will automatically display as “GND”.

  4. This will now automatically serve as an inner layer.

  5. Anything you draw on this layer actually removes copper instead of adding it.

Greetings Daniel,

Something’s wrong here. How are you creating a new layer? If you type ‘Display’ or hit the icon for the layers what do you see?

Depending upon the version of EAGLE you may only have two, four or all sixteen layers. The standard version does four layers and these are:

Top

Route2

Rout15

Bottom

The student version only has top and bottom, the pro version has 16 (I’mnot sure if you see then all at once or need to add them).

Daniel Wee:
Well I’ve done all this but for some reason, the GERBER files that the CAM processor generates for this layer is empty. Am I missing something here? Any help will be greatly appreciated.

What CAM job are you using to extract the Gerbers? I think SFE has a four layer job in addition to the two layer that I have used.

Comments Welcome!

4

Ahh… I see. I’m using the free version of Eagle PCB. Am I to understand then that this version will not support inner ground planes?

Daniel

5

The free version does not support more than the top and bottom layers.

6

Okay, so now I’ve gone and bought the Standard version but I still can’t get the supply layer to work.

When I create a new layer, it starts with layer 100 or there abouts. So I name the layer $GND (my ground net is called GND). Now, if I view the created layer, it will have the supply layer option checked but grayed out. The problem is I can’t seem to see anything in this layer.

Daniel

7

Daniel Wee:
Okay, so now I’ve gone and bought the Standard version but I still can’t get the supply layer to work.

When I create a new layer, it starts with layer 100 or there abouts. So I name the layer $GND (my ground net is called GND). Now, if I view the created layer, it will have the supply layer option checked but grayed out. The problem is I can’t seem to see anything in this layer.

Greetings Daniel,

Congrats on your new purchase!

Can you open the Control Panel → Help → Product Information

and tell us what rev you have installed?

Next, download this

[schematic

and this

[board

and open them in EAGLE.

This is a junk project test file with two layers and polygon fills

that I use for checking EAGLE operation. In the board editor

click on the Ratsnest command (or just type Ratsnest on the

command line). The power and ground planes should fill in

blue and red respectively.

Next, go to the Display command (or just type Display on

the command line). Look at the lowest number layers, you

should see four signal layers (Top, Route2, Route15, Bottom).

Report back here when you get to that point.

Comments Welcome!](http://www.stonard.com/SFE/eagle_test.brd)](http://www.stonard.com/SFE/eagle_test.sch)

8

Okay, thanks guys. I got it sorted out. As it turns out, you need to use layers 1 to 16 for your signal layers. And using Layer 15 for ground did the trick. For some reason using layer 3 didn’t quite work.

Now I have it so that 1 and 16 are the top and bottom layers, and 15 is the ground plane, and 2 is an internal routing layer. Everything works except for the DRC which complains that the stuff on layer 2 has the error “Layer Setup”. I am guessing that this is related to the DRC Layer configuration which is currently (1*16) but don’t know how to solve this. Will be checking on this now.

Again, thanks guys.

Daniel

9

Daniel Wee:
Everything works except for the DRC which complains that the stuff on layer 2 has the error “Layer Setup”. I am guessing that this is related to the DRC Layer configuration which is currently (1*16) but don’t know how to solve this.

Daniel,

Good guess. Open the DRC dialog (in the board editor window) or

type “DRC”. Select the layers tab. EAGLE is asking for guidance on

how the multi-layer PCB is constructed. A two sided is easy -

only one core with cu on both sides. With more than two layers

there are two or more cores separated by prepreg.

EAGLE wants to know if the vias go through all layers or are

‘blind’ layer to layer internally. I think blind vias can only

go through internal cores, not prepreg.

The default for two layers is (1*16) as you noted.

For BatchPCB four layer I would guess it’s (12) + (1516).

This gives four layers and three spaces, you may adjust the

spaces in the dialog box on the layers tab. I would assume

all three are equal. Also, that internal layer copper is the

same thickness as the outer layers.

Try it and perhaps somone that has done a four layer EAGLE

PCB through BatchPCB can confirm?

Comments Welcome!