Thru-hole component an via connecting to internal layers

[Anonymous]

In a previous software I was using a 4layer design with the following setup. signal/gnd/vcc/signal.  I was able to connect to the inner layers on all thru-hole and via. No blind or stopped via.  Am I able to do this in Eagle?

[one-of-the-robs]

Yes. Obviously.

[Anonymous]

I have only had eagle for a couple of weeks and will be trying to do a
6layer board. So it is possible, how is it done. the software I was using
you could right-click for a properties choice on the thru-hole or via and
choose what type if any connection to an internal layer. I could not see
any way in the drc to set this up., thank you

[one-of-the-robs]

All PTH pads and full vias have connections on all layers by default. The DRC lets you set up smaller annular rings on inner layers to avoid "wasted space" (although the clearance from a track to the ring probably doesn't really restrict you any more than the clearance to a hole would).

You can route to or from a via on any layer, just by choosing the layer in the routing drop-down. The Autorouter (which I would recommend you DON'T use until you really know how to drive it, and even then don't use it much) will route to or from vias on whatever layers you permit it to use.

If you have a via or PTH pad connected to a net that has a polygon flood on a layer (any layer) then Eagle will connect the flood to that via or pad.

In other words, don't get hung up on "inner" vs. "outer"! With a few exceptions (such as the different annular ring settings in the DRC), all layers are equal to Eagle. There is no need to faff around with having to specify whether to believe in a layer on a per-hole basis, like your other tool forced you to. That sounds horribly inconvenient to me.

[Anonymous]

FOR EXAMPLE, i HAVE A CONNECTOR THAT SUPPLYS POWER TO THE BOARD. THE INNER
LAYERS ARE LAYER 2, GND FULLY PLATED AND LAYER 3 IS +12v ALSO FULLY PLATED.
WITHOUT USING STOPED OR BLIND VIAS, HOW DO i DESIGNATE CONNECTION OF THE
CONNECTOR TO DESIGNATED LAYERS. ALSO i HAVE AN OP-AMP THAT REQUIRES SOME
OF THE RESISTORS AND CAPS TO CONNECT TO THE GND LAYER AND THE OPAMP TO
CONNECT TO +12v. HOW DO i SET IT UP TO SHOW THIS IN A MANUAL ROUTING. THE
DRC shows me I can set up blind and stoped vias, but I do not see how to
set up a PTH that would connect only to one of the inner layers. Also how
do you designate a layer to be a netlist name such as gnd or Sig.(probably
not right terminology.
Thank you

[one-of-the-robs · Accepted solution]

You're over thinking and looking for problems that just aren't there!

I don't know what previous software you used or what convoluted hoops it demanded you jump through, but with Eagle all is easy.

So you have a connector, which has a pin on the schematic connected to a net called +12V. On the board you have a full polygon on layer 15 which is named +12V and therefore is connected to the net called +12V. Eagle will connect them if it can. There will be a connection, on layer 15, from the polygon to the pad (PTH hole).

I don't recommend relying on that, though, for a number of reasons all hanging round polygon fill being unreliable. You should route your power and ground explicitly and manually. That's also easy. Start the route tool, select layer 15 in the drop-down, click on the connector pad then route it out to the other places you need to connect to. The route will be on layer 15 and all the necessary connections are made.

A PTH for a component pad will ALWAYS pass all through the board, and will have plating present on all layers. You can route to or from it on ANY layer.

Forget about blind or buried vias. Just don't go there. They add cost for negligible benefit and you don't need them unless you're designing a ten layer board with BGA devices.

Any hole that goes through the board must pass through all layers (simple geometry!) and if it's plated it will have plating on all layers (again, geometry). Eagle will always add a (probably tiny) ring of copper round it. If you need to connect to it, Eagle lets you connect to that ON ANY LAYER. If you don't want to connect to it, Eagle adds a clearance ring to any polygon fill (or explicit supply layer, although those are deprecated if not obsoleted) on any layer.

To designate layer 2 as your ground plane, put a polygon across the full board on layer 2 and name it GND. Simples.

And READ THE MANUAL. This is all in there.