Two layer PCB throughhole with copper on bottom only

[Psi]

Hey,

Is it normal to have a two layer PCB were some of the through hole pads are only on the bottom layer?

I ask because I'm designing a two layer board and for some of the through hole components pads i want copper to be only on the bottom layer (not the top).
Obviously with copper only on one side these pads cant be plated through.

In Altium if i change these pads from multilayer to bottomlayer it seems to do exactly what i want.

But my question is..
Is this normal?, do i need to make a point of telling PCBCart about these pads being different or is it perfectly normal to have some pads like this on a two layer pcb?


The reason for wanting this is because the top layer has some large text printed on it. A few holes in the text will look fine but big shiny gold pads will ruin the text.
(The boards are duel use, some have 5x7 led matrix arrays soldered in over the top of the text, others don't and the text is visible instead)

[joelby]

I doubt it'll be a problem. You might want to include a read me file that states that some pads are only on the bottom layer and that these should not be plated through.

In my experience, PCBCart are pretty on the ball and will query things they're not sure about.

[tycz]

Obviously with copper only on one side these pads cant be plated through.

The PCB manufacturer will certainly be able to plate through a hole with a pad on one side only. It's common practice for mounting parts like crystals which have metal bodies.

[Psi]

Obviously with copper only on one side these pads cant be plated through.

The PCB manufacturer will certainly be able to plate through a hole with a pad on one side only. It's common practice for mounting parts like crystals which have metal bodies.

interesting, i thought the electroplating process required a pad on each side to act as the electrodes.
Though, that was probablby just an assumption on my part.

[johnmx]

It’s possible to plate a hole even without pads. E.g. set the annular ring as zero (PAD size the same as the hole) and you will get that.
Usually you must define all non-plated holes in a separate drill file, see the manual of your PCB software for details.

Electroplating process (with video):
http://www.eurocircuits.com/index.php/making-a-pcb-eductional-movies/44-plating

[Short Circuit]

When the PCB is plated, their is still copper on the entire PCB surface, so it is not possible to prevent a hole from being plated.
Also, it is not really possible to have a plated hole without pads on both sides. There is always a little bit of annular ring required,
but this can be very small, depending on process tolerances as little as 0.1mm, so barely noticable.

As been said, non plated holes require an additional tooling process after the etching and plating process. Therefore you need
an additional drilldata for non-plated holes (or a single file having sepearate entries for PTH and NPTH).

[johnmx]

Also, it is not really possible to have a plated hole without pads on both sides. There is always a little bit of annular ring required,
but this can be very small, depending on process tolerances as little as 0.1mm, so barely noticable.

I have to disagree with you. It’s possible to have a plated hole without pads. Why? Because I have the proof in my hands!
The only visible metal area is the plating thickness which is 35um and that’s not really a pad.

[Short Circuit]

The first photo looks more like a non-plated hole to me.

And yes, you can be lucky and get away with it. But don't do it if the plating is important.
Also, most PCB manufacturers with decent dfm checks will comment on such holes.

However, after checking the production steps at http://www.eurocircuits.com/index.php/making-a-pcb-eductional-movies ,
I must agree that there doesn't seem to be a technical reason for not allowing this.
(But can't think of a reason to want it either.)