What are Castellated Holes?
Castellated Holes (a.k.a. Plated Half Holes, Castellations, … ) are a series of Plated Through Holes or Vias placed on the edges of the PCB and allow you to transform your PCB into a surface mounted sub-assembly. When cutting the board at the end of the manufacturing process, only a half of each plated hole remains in the PCB. These Plated Half Holes now serve as pads to solder the sub-assembly to the surface of the motherboard.
Which designs of Castellated Holes does AISLER support?
AISLER supports the half hole technique mentioned above - it is the easiest and most common way to design Castellated Holes. Please follow our design rules in the next section to get the best results.
How to design Castellated Holes?
Integrating Castellated Holes to your PCB is very easy. Just make sure to pay attention to the following points:
- Place the center point of every castellated hole exactly on the edge/ board outline of your PCB. It is important that these holes are plated-through. They must be included in the drills-layer.
- Always use the top and/or bottom edges as locations for your holes! Do not use the vertical edges (left and right), because they are predominantly used for our bridges to hold the PCB in place. See also our article about (Bridges and Frames).
- The copper-layer should have pads while the soldermask-layer should have openings.
- Minimal drill hole diameter: 1.0 mm (0.04 in)
How does it work?
If your PCB matches our design requirements, we will remove a small area of the copper-layer. This way we ensure, that the edges of your PCB get the necessary high quality for mounting/soldering it on your motherboard.
Thank you for the information.
I have a related question but I cannot find any answers in the forum.
It would be great if you could answer it.
- How about side plating. Does Aisler support outer and/or inner side plating? If so, what are the specifications?
- The minimal 1mm diameter of castellated holes refers to the drill hole diameter or the minimum pad diameter? (assuming the pad is concentric circular)
Your clarification is much appreciated.
welcome to the community!
- Right now we do not support side/ edge plating.
- The minimum diameter refers to the drill hole diameter, not the pad. (I will clarify this in the description!)
Is it possible to have castellated holes on the edge of a cutout of the board outline, as long as I keep to the top/bottom edges?
For example, like this:
Hi @flx ,
Welcome to the community!
Is it possible to have castellated holes on the edge of a cutout of the board outline […] ?
Yes, it is!
[…] as long as I keep to the top/bottom edges?
In principle, you can also place castellated holes on all other edges. Just be aware that they may conflict with our bridge positions.
If your board is small (height + width < 60 mm), you are on the safe side with the top or bottom edges of the outline. For all other cases, it makes sense to think about using user-defined bridge positions (see also Bridges and Frames).
I’m currently working on a relatively large module with castellated holes (90.0mm x 80.0mm). According to the previous posts I assume that the five half holes on the right side (see image) are not an issue – I have to have a custom frame anyways (I could add some more tabs on the sides though).
However, what concerns me a bit is the length of of the castellated top and bottom edge. Do you think this board would be manufacturable or should I add tabs to these edges? If that is required: How many would you suggest?
Welcome to the community!
According to the dimensions of your board - width & height >= 80.0 mm - you’ll need eight user defined bridges in total.
With a width of 90.0 mm, I think it is still acceptable not to place bridges on the top and bottom edge. (For much longer edges, however, you certainly have to handle it differently.) It should be sufficient if you distribute the eight bridges on the sides, e.g. as shown in the picture below.
Thank you for the quick reply
Hi, I have to make a PCB with castellated Vias on all four Edges, however, there should be sufficient place for connection Tabs in the corners of the board.
In the PCB Rendering your engine seems to recognize the castellated vias just fine, however, what worries me is, that the copper of the pads does not go to the edge of the board. Shouldn’t the copper of the Pads go all the way to the edge when it’s a castellated via? Am I doing something wrong here?
I think they do that to make cleaner contacts possible. When the copper goes all the way to the edge, it frays unsightly.
Hi @Techko ,
don’t worry, that’s exactly how it should look like!
@andreas-eet has already provided the correct answer here: By setting back the copper, we try to reduce copper burrs / leftovers as much as possible.