hole and via same thing?

[Munib]

how do you pick a via size

I m very new to PCB designing
I got confused about these terms
Hole , Via , Drill bit size
Are they same or different?
define and explain

 

[shamrani]

via between two internal layers or upper (bottom) side and internal layer.

hole between the upper side and bottom side of the pcb

 

[House_Cat]

Let's start with drill bit size - that is the size of the drill that the PCB fabricator uses to drill holes in the PCB for mounting holes, vias, and thru-hole pads. They come in standard sizes, so you can't specify just any hole size and expect the fabricator to be able to make it - the hole has to match the available drill sizes.

If you are specifying hole sizes on a PCB, you normally specify "finished" hole size, not the drill size. The finished size of a via hole or thru-hole will be smaller than the drill size. The reason is the copper plating that will be done inside the drilled hole to make the connections to the various layers of the board. Usually, but not always, the finished, plated, hole size is about 2-4mils smaller than the drill size because of the copper plating.

The size of the hole you put in a via or pad is dependent on whether or not you need to solder a lead in the hole, the available space, the frequency of the signal passing through the plated hole, the current, etc. As the designer, you tell the fabricator what size you want the hole when it is plated. The fabricator picks the drill size that will make a hole big enough to give the finished size you want after plating. As designer, you also have the responsibility to make sure that there is enough pad or via diameter to allow the fabricator to choose his drill. If you specify too big a finished hole for the pad size, the fabricator's drill will remove all the pad or via copper. Normally the fabricator's specifications tell you what minimum "annulus" he needs remaining on the pad or via after drilling to ensure he can properly plate the inside of the hole.

The term "via" means a connecting plated hole between two layers. Vias can connect top signal paths to bottom signal paths or they can connect signals on any two other layers. A special case of a via is a "blind via". The blind via doesn't go all the way through the board. It connects two symetrically spaced inner layers together, but doesn't go all the way through to the top and bottom. They are made by drilling and plating holes in the early stages of PCB fabrication as the board layers are laminated to the core in opposing symetric pairs.

"Thru-hole pads" are the same as vias but are usually associated with components - for example the pads for a resistor with leads, a capacitor with leads or an IC with leads. They can also be single "free" pads that connect traces layer-to-layer like a via (free means that it isn't part of a component). From the standpoint of terminology, pads aren't restricted to connecting only two layers like a via. A thru-hole pad can connect on any or all of the layers that it passes through. For example, if I wanted to connect a trace on the top layer to traces on inner layer 2, layer 6, and the bottom layer - I would use a free thru-hole pad. If I wanted to connect a trace on the top layer to a trace on just inner layer 2 - I would use a via.

The distinction between a free pad and a via is just terminology. They are both used to connect between layers. Your PCB editor software is probably programmed to allow a via only to connect two layers, but it will allow a thru-hole pad to connect many layers.

 

[smox]

yes, they are them same thing.

 

[taring77]

initially i was also confused when i started desining

Hole - it could be some thing that is thru from one layer to another just like an ordinary hole that if u take one laye u can see thru

Via - there are blind via and buried via and thru hole via.
its the one that connects one electrical later to another thru this and making a hole
20/10 via size. the via is 10 mils while its plated with gold plate and makes the whole smaller

i've heard of plp calling it via hole too


Drill bit size - its the size of the drill bit that is use to make the hole of ur via on the board.


regards
taring77

 

[Johnson]

House_Cat,
Would you begin a talk on mounting technology, and related design consideration.
Let's start with a simple one, what is the mounting guide? For automatic mounting which information must be available on design?

 

[House_Cat]

Would you begin a talk on mounting technology, and related design consideration.

Wow! - lengthy subject to discuss in just a few lines on a forum.

There are several companies that make automatic mounting, or pick-and-place machines. Each of them has their own format requirements for pick-and-place files. A pick-and-place file has x-y position information, and rotation information, for each of the components on a PCB.

One thing that all placement machines have in common is the need for some way to target (or precisely locate) the footprint on the PCB. The way this is done is to place a "fiducial" near the more complex surface mount devices, such as multi-pin ICs. A fiducial is a dot of copper placed on the board by the PCB designer that allows the placement machine operators to target their machines using an optical sight.

The layout and description of the fiducial mark is described in the document attached.