Add holes for through hole components

Angela Ameruoso wrote:

Hi, I am new in the Eagle world and I am making a 2 layers custom board with Eagle. 

I am trying to do a simple custom size board full of holes for through

hole components ( a simple prototyping board) and I am not sure about

which is the best way to make the holes.

depends 8-)

for pads that need a connection in the schematic you can use

wirepad.lib parts.

They need to be i nserted in the schematic.

But for the pads without connections, use plain vias.

They are inserted/placed in the board only.

You can still connect this vias with the connect command (in the board

editor - to form a GND rail for instance)

--

Lorenz

Lorenz wrote on Thu, 02 March 2017 06:59

But for the pads without connections, use plain vias.

They are inserted/placed in the board only.

You can still connect this vias with the connect command (in the board

editor - to form a GND rail for instance)

Are you sure? I thought the connect command was used in the library editor

to connect pads to pins in a part? I think in this case you'd want to use

the name command to name any vias you wanted to be connected together to

the same net or simply add them with a name already set.

e.g. name 'GND' or via 'GND'

I'd suggest that if you really wanted any of the holes connected you'd want

to have a schematic and connect them there though rather than doing it all

in the board so if this was the case the wirepad.lbr option would probably

be the correct option.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

Hi Angela,

Holes, pad:
Well, in the schematic or pcb you have 3 types of holes (round eg drilling, square eg punching, complex eg milling) that are separated into plated or non-plated holes.

A via yes is, of course, also a plated hole, but its using is a bit different.

In the schematic - ADD from the library, you can choose from:

Holes.lbr (mounting holes, non plated or plated, round or square, or even complex special hole)
Solpad.lbr (solderable pads, but this lbr is very inflexible)
Wirepad.lbr (solderable pads, through holes with type of hole diameters and rings, also SMD pads)
Or you can create your own lbr file with your pads or holes.

If you use ADD in pcb i strongly suggest that you imports just holes, but not pads if they are will connected to an electrical contact.

If you likes importing pads then make this into the schematic, also better importing the holes into the schematic.

(-> consistence between schematic and pcb)

The point:
PAD is basically a plated hole or a SMD pad
HOLE is basically a non-plated hole, is only for assembly or for the distances, e.g. for high-voltage security distance.

For your project I suggest you to make your own lbr file. You can also copy the default pads into your lbr file.
Please also read the manual and the tutorial. There you will find nice examples.

Via:
A plated hole used in the circuit board to connect through and between the layers.
They can also be very flexible.

If you want to connect some of the vias to a wire, you must use the command: NAME

Then the menu will ask you: "this segment or complete wire" -> use complete wire!

Power plane:
Power planes are usually created by drawing a polygon, and then this polygon will connected to an electrical wire.
(E.g. GND or VCC or VDD, .... or N $ xxx

-> and if pads or vias are connected to this wire, then the polygon includes it in its calculation.

Best Regards,

Gerald

---

If the pads are going to be isolated for a prototyping board, try placing test points with the desired pads on your schematic and then placing them on your PCB.

If needed make your own test point component.

Thank you all.

I am not importing nothing from the schematic page because I don't have other components on the board, just holes and a brand logo, so I am making directly the board in the board page of Eagle.

For a bettere understanding, I am making this simple type of board (see figure below) but with a custom size and a logo.

There are many ways to do it. The one in this photo was created by making a component for the pads. To simplify further I created a component that was a block of pads (e.g. 4x4 or whatever).

Hi,

ok,,, in this way you can create your board as a component in the library.

Because if you place the pads in the schematic then you can have a lot of work to sorting that on the pcb.

But as a component you'll place it all directly on your defined place and they will stay it on there.

Then you can draw the logo in the symbol of this pcb.

Just make a defined number of pads and place it as group where ever you like.

Gerald

---

It is always best to schematic capture a PCB because it allows revisions and additions to it to be easily accomplished.

For example - your Proto board - There will most likely be a stage where you want to add power rails or planes to it.

Facilitating this is done easily using a schematic.

There's no reason why you can't capture the prototyping area as components and have them placed on your PCB.

If fact EAGLE works best in this mode because it switches between its schematic and PCB for its Design Rule Checking.

I just kluged this up in moments to illustrate the point. Complete with mounting holes.

The size of this board is at the maximum freeware limit.

It also makes for a good familiarisation practice session with EAGLE for Library, Schematic and PCB editing.

If you look very closely you'll also see the two pads with the enlarged holes as per your photo.