Perfect annular ring size for given lead size when datasheet does not exist?

I have a round component lead.

The component lead is 6.2 mm ±0.1 mm.

I need a hole for this lead that is big enough. The capability of the PCB manufacturer is +/-0.2 mm for holes. The hole for the lead will be plated.

Should the hole size be 6.2 mm + 0.1 mm + 0.2 mm = 6.5 mm, or should I add 0.1 mm since it is a plated hole?

I need an annular ring for the lead. This lead might be under some mechanical stress. I have room on the board, so I want to have the ideal size of the annular ring.

• How do I calculate the best annular ring size?
• Is a bigger annular ring size always better?
• Could I, for example, have a 3.25 mm annular ring? That's the maximum I can fit on this PCB.

Is there a formula a given lead size/hole size to calculate the perfect annular ring?

This is for a component that is specially made, so I have no datasheet specifying the information regarding the best footprint. Quite some current (maybe 20-60 A) will go through the lead.

• The bigger the annular ring, the better its adhesion to the board. If you can fit a 3mm ring and it's not a problem for your soldering process, go for it. There aren't really any downsides. Commented Nov 17, 2022 at 9:55

So the hole size should be 6.2 mm + 0.1 mm + 0.2 mm = 6.5 mm. (Correct? Or should I add 0.1 mm since it is a plated hole?)

You don't have to. Because the hole size for plated holes (PTH - plated through hole) will be taken as "finished hole size" for the manufacturer. This means that a 6.5mm PTH seen in your gerber will be drilled with 6.6~6.7 to have 6.5mm after plating.

How do I calculate the best annular ring size?

There's no universal best annular ring size. It depends on a few factors:

• Physical properties of the component (Larger/heavier components, unless supported with extra things such as glues or holders, are attached to the PCB from only to the pads. And because of that, if there's a high chance for bending then the chance of losing/damaging the pad increases)
• Production methods (hand-soldering, wave soldering, etc.)
• Hole type (PTH or NPTH) - Annular ring around an NPTH generally comes off easier during manual work or servicing.
• Teardrops should be considered.

Is a bigger annular ring size always better?

Generally yes but in case of manual soldering bigger ring means longer time to heat up.

Could I for example have a 3.25 mm annular ring (the max. I can fit on this PCB)?

The distance to adjacent pads/holes/rings and their sizes should be considered. In case of wave soldering larger rings collect larger solder, so if there's a considerably small pad (e.g. 1mm-dia) at a very low distance (e.g. 0.3mm) then there's a chance of having short-circuits.

IPC-7251 calls out standard specifications for through hole design. It describes how to calculate hole diameter and pad diameter for given lead dimensions. Check out this link here:

Minimum Hole Size is calculated according to equations below:

Minimum Hole Size = Maximum Lead Diameter + 0.25mm (for Level A of IPC-2222)

Minimum Hole Size = Maximum Lead Diameter + 0.20mm (for Level B of IPC-2222)

Minimum Hole Size = Maximum Lead Diameter + 0.15mm (for Level C of IPC-2222)

After you calculate the Minimum Hole Size, you should know that the Minimum Annular Ring is 0.05mm (50um). According to IPC-2221 the Minimum Fabrication Allowance is 0.6mm for Level A, 0.5mm for Level B and 0.4mm for Level C.

Pad Diameter = Minimum Hole Size + Minimum Annular Ring X 2 + Minimum Fabrication Allowance

Pad Diameter = Minimum Hole Size + 0.1mm + 0.60mm (for Level A of IPC-2221)

Pad Diameter = Minimum Hole Size + 0.1mm + 0.50mm (for Level B of IPC-2221)

Pad Diameter = Minimum Hole Size + 0.1mm + 0.40mm (for Level C of IPC-2221)

Example: Maximum Lead Diameter = 0.55mm

According to Level A Minimum Hole Size = 0.80mm; Pad Diameter = 1.50mm

According to Level B Minimum Hole Size = 0.75mm; Pad Diameter = 1.35mm

According to Level C Minimum Hole Size = 0.70mm; Pad Diameter = 1.20mm

Here is what that page says about the three levels used above (A, B, and C):

Levels A, B and C describe the measure of the relative ease of manufacturing.

Density Level A is used for General Design Producibility. It is a Preferred Level. Level A is used for the Low component density. In this case, footprint geometry is ‘Maximum’. This method is applied to the most robust producibility.

Density Level B is used for Moderate Design Producibility. It is a Standard Level. Level B conditions are suitable for reflow, wave, drag or dip soldering. In this case, footprint geometry is ‘Median’. This method provides a robust solder attachment conditions.

Density Level C is used for High Design Producibility. It is a Reduced Level. Level C is used for the High component density. In this case footprint geometry is ‘Minimum’. This method is applied to a hand-held and portable appliances.