IPC-2221 & 2222 and Through-hole Pad Stacks

The leading document for PCB fabrication is IPC-A-610. IPC-610 is used by most PCB fabrication shops to manufacture PCB’s for their customers end-use, which are broken up into 3 Classes, 1, 2 or 3.

CLASS 1 – General Electronic Products

Includes products suitable for applications where the major requirement is function of the completed assembly. Toys

CLASS 2 – Dedicated Service Electronic Products

Includes products where continued performance and extended life is required, and for which uninterrupted service is desired but not critical. Typically, the end-use environment would not cause failures. Computers & Phones

CLASS 3 – High Performance Electronic Products

Includes products where continued high performance or performance-on-demand is critical, equipment downtime cannot be tolerated, end-use environment may be uncommonly harsh, and the equipment must function when required, such as life support or other critical systems. Military & Medical

This affects the CAD library Through-hole packages due to the pad stack construction must meet or beat the IPC-610 rules for Annular Rings, Plane Clearance, Inner Layer Pads, Thermal Relief Patterns as shown below.

There are not many IPC-610 Fabrication rules for Surface Mount Technology. Minimum pad to pad & solder mask swell for registration might apply. But the pad size and spacing are most important for the Assembly process for component attachment guidelines identified in the J-STD-001 standard.

When defining a pad stack, you first must define the hole size. This is done by taking the maximum lead diameter for round leads and the hypotenuse of a rectangle shape lead. IPC considers that both round and rectangle leads are the same, but PCB Libraries, Inc. believes that the round terminal lead consumes more volume in the hole than a rectangle lead and therefore the hole over round lead should be larger than hole over rectangle lead. Library Expert allows the user to change both values independently. The Library Expert Preference default values are Round Lead + 0.20 = Hole Size and Rectangular lead + 0.15 = Hole Size.

However, IPC-2222 has a table that is inclusive and calculates the hole size based on Density Levels. See image below.

Once the Hole Size is established, the main point for pad size calculation in the IPC-2221 standard is the minimum annular ring of the plated through-hole pad stack after fabrication tolerances are applied. Here is an image of the minimum annular ring.

There are 2 fabrication tolerances that must be accounted for. The first and most obvious one is the hole size tolerance that is in the drill chart on the fabrication drawing. The typical hole size tolerance for a through-hole terminal lead is +/- 0.075 mm (3 mils) and vias are + 0/- Hole Size. If the minimum annular ring for an external plated through-hole is 0.05 mm (2 mils) and the hole size tolerance is 0.075 mm, the pad size annular ring must be 0.125 mm or a pad size of 0.25 mm over the hole size.

The second tolerance that needs to be applied to calculate the pad size is the layer to layer registration. This is typically held to 0.075 (3 mils) and only occurs when the layer count is greater than 4 layers. A 10 – 20 layer PCB could have layer to layer registration issues in every direction on the inner layers. The minimum annular ring on the inner layers is 0.025 mm. For Class 3 boards that are 10 or more layers, the maximum layer to layer registration should be held to +/- 0.05 mm. Also, the hole tolerance should be set to +/- 0.05.

Let’s make it simple. 0.025 minimum annular ring + 0.05 layer to layer registration + 0.025 hole tolerance = 0.10 annular ring or the pad size = 0.20 over the hole size. But if the fabrication shop cannot hold the layer to layer registration to 0.05 mm and requires 0.075 mm, then the minimum pad size would be 0.25 mm over the hole.

All of these values can be set in the Library Expert software Preferences to ensure that your through-hole calculations meet or beat your fabrication tolerance allowances.

The via hole quantity typically out numbers the terminal lead holes and PCB designers want to make the via annular ring the minimum value per the manufacturing Class that they must meet. Since there is no terminal leads in a via hole, the hole size tolerance can be + 0/- Hole Size. Allow the fabrication process to plate the via holes closed. If an inner layer shifts 0.075 in any direction, the annular ring is affected. See the image below.

Another important pad stack calculation is the plane anti-pad. Most fabrication shops require a minimum annular ring of 0.35 mm (15 mil) over the hole size. Making the plane anti-pad annular ring smaller could cause the drill hole to be too close to the copper plane and making it larger removes important plane copper that carries the signal return path for transmission lines. Ideally, the plane anti-pad would be smaller than the pad size + the electrical clearance. The electrical clearance is the trace to pad spacing rule. All traces on all layers should be over a copper plane and not intrude into the anti-pad area. Therefore, make the anti-pad large enough to manufacture but small enough to maintain signal integrity.

Note: The OD of the plane Thermal Relief is the same diameter as the plane Anti-pad.

Incremental pad sizes are important for a couple reasons. Small through-hole components have small terminal lead diameters that require smaller hole sizes. Small packages are normally light in weight and they don’t carry much current. Parts that require higher currents need larger terminal lead diameters. High current parts generate more heat and are heavier in weight. These features require a more robust annular ring that will allow more solder to hold the part in place and to handle the heat transfer. The Library Expert software program uses a default multiplier of 1.5 X hole size for the pad size calculation. See the image above for the pad size calculation with a 1.0 mm hole verses a 2.0 mm hole. The annular ring doubles in size.

All of the pad stack calculation values in the Library Expert software program come default with the best-known industry practices, but they are all user definable to ensure that your plated through-hole calculations meet or beat your corporate or customer standards.