4

I'm writing to make sure my process is correct in this design. I'm going for a standard 4 layer board with layers 1 and 16 as signal layers, and layers 2 and 15 as VCC and GND layers respectively. I have filled layers 2 and 15 with the necessary polygons and names them to match the schematic. My only question really deals with the design of the layers and the use of vias (see picture). Is this the best way to accomplish my goal here? I am dealing with a relatively dense circuit as size needs to be kept down (insect cybernetics). Could I get some second opinions? This seems to be the best design.[My settings[1]

I want to be able to connect to the vcc and groun planes from the top level only. This setup has allowed me to select the layer combinations I was looking for with my vias.

Thanks everyone.

EDIT/UPDATE

After reading what ThePhoton says I tried a new approach by eliminating the blind vias and instead using a more conventional 4 layer board setup. see here

And for via settings I simply renamed its net. Will this give me the desired effect? enter image description here

Donald O'Boyle III
  • 41
  • 3
  • What CAD tool are you using? I find it unusual that you have layers numbered higher than "4" in a 4-layer board. – The Photon Oct 04 '18 at 21:31
  • 6
    Blind vias are incredibly expensive. You should change your design to use vias that go through the full board thickness if possible. – Dwayne Reid Oct 04 '18 at 21:32
  • I'm using Autodesk Eagle. I agree that it is weird however eagle assigns the bottom layer of the board as "16" by default so I stuck with this convention. – Donald O'Boyle III Oct 04 '18 at 21:32
  • @DwayneReid Could you suggest a way to get the flexibilty of seperate GND and VCC layers without the cost of blind vias? – Donald O'Boyle III Oct 04 '18 at 21:33
  • 2
    You can still have GND and VCC layers. Just don't connect to the vias on the layers you don't want to make a connection to. The CAD tool will automatically make an "antipad" around any via through a plane layer that isn't meant to connect to that plane. – The Photon Oct 04 '18 at 21:34
  • @ThePhoton Well that's good to know. In that case how do I access those layers otherwise? Before I just had one through hole via and when I tried to connect any via I create to a respective GND or VCC plane it would only list "1-16" (a signal path from top to bottom layer). Would you be able to give me a more descriptive procedure to employ your method? – Donald O'Boyle III Oct 04 '18 at 21:37
  • 2
    If you assign your via to the VCC net, it will connect on the VCC layer. Otherwise it won't. If you want to route signals on those layers, you probably have to make them signal layers instead of plane layers (but I don't use Eagle, so don't know the details of how to change it). – The Photon Oct 04 '18 at 21:39
  • Thanks for the heads up @ThePhoton, I believe I have used your tips correctly. – Donald O'Boyle III Oct 04 '18 at 21:44
  • With CAD systems I've used, just placing a via will make a via not connected to any net. To get a net connection on a via (or track) you have to place the via on a track that already has the desired net name, or start a track from something on the desired net, and place the via as part of the "place track" process. – Peter Bennett Oct 05 '18 at 00:37
  • In Eagle, place the via and then use Name to set the net name for the via and route tracks from there. When the polygons are repoured, they will connect to or be separated from the via automatically as appropriate. – Dean Franks Oct 05 '18 at 01:11

1 Answers1

7

Though you already got your answer:

Better 2-layer PCBs are made of fiberglass mats soaked with resin. The resin is hardened, the whole thing is plated with copper, and you have your raw PCB.
During production of an actual board, it is drilled two times: First for all vias an through-hole component pads. They are then chemically plated with metal to make them conductive. Second, at some time after the plating process to make mounting holes etc without plating.

A 4-layer PCB is actually two 2-layer PCBs (cores) glued together by an other layer of soaked fiberglass (prepreg), which is hardened after. This is what your pictured show: Two green cores with the prepreg inbetween.

It is easily possible to create vias from one side of a core to the other, as this is the same as for 2-layer PCBs. But it is costy, since it is an extra step in production. But it is very difficult to create vias through a core and a prepeg, bu not the next core, as the second via style in your image shows. One had to drill to a certain depth into the board, and plating a blind hole is difficult to impossible.

Finally, it is much cheaper to have normal vias going through the entire board, and many manufacturers, especially pooling services, only offer these vias.

There are also very few manufacturers which etch a center core, apply a prepeg on both sides, plate it with copper and then etch the outer layers. And more-than-4-layer boards are made alike. This has different constraints for vias, but you got the point.

For designing in EAGLE:

A ground plane is a polygon typically with name GND. Place a via, and the ground plane will get a cut-out to not touch the via. Name the via GND, and the ground plane will connect to it. During routing of a signal which is already named GND, any of its vias are automatically connected to the GND plane.

sweber
  • 8,580
  • 1
  • 15
  • 35
  • Thank you for your in depth response @sweber. So if I create this ground polygon on layer 15 my vias will still connect to it? or should I make my polygons on layers 1 and 16? – Donald O'Boyle III Oct 06 '18 at 03:18
  • 1
    Yes, a via or pad will always connect do a copper polygon, regardless of the layer number. – sweber Oct 06 '18 at 12:15