See the Blue print on Launchpad: https://blueprints.launchpad.net/pcb/+spec/padstacks

Hereafter follow some copy/paste snippets I found regarding padstacks and a naming convention.

The Padstack Naming Convention consists of combinations of letters and numbers that represent shape, or dimensions of lands on different layers of printed boards or documentation. The name of the padstack needs to represent all the various combinations. These are used in combination with the land pattern conventions defined herein according to the rules established in the IPC-2220 Design standards.

The first part of the padstack convention consists of a land shape.

There are eight basic land shape identifiers.

Note: All alphabetical characters are “lower case”.

This helps discriminate numeric values.

Illegal characters that cannot be used (Microsoft requirement) include “ ” , ; : / \ [ ] ( ) . { } * & % # $ ! @ ^ =

Basic types:

h = Plated through hole

n = Non-plated through hole

v = Via (can be blind or buried)

Basic Land Shape Letters:

e - Ellipse shape

c = Circular shape (a specific kind of ellipse)

r = Rectangle shape

s = Square shape (a specific kind of rectangle)

b = Oblong shape

u = Contour shape (Irregular Shape)

d = D shape (Square on one end and Circular on the other end)

o = Octagon shape.

Examples utilizing the padstack naming convention (all values are in metric units)

Note: Every number goes two places to the right and as many as needed to the left of the decimal

Examples: 1150 = 11.50 mm or 11500 μm, 150 = 1.50 mm or 1500 μm, 15 = 0.15 mm or 150 μm.

This leads to one unit being 1/100th of a mm, or a centi-milimeter ... a [cmm] 😉

c150h90 where "c" denotes a Circular land with a 1.50 diameter and "h" denotes a hole size of 0.90 mm

v50h25 where a "v" denotes a via with a 0.50 mm land (default Circular land) and "h" denotes a 0.25 mm hole

s150h90 where "s" denotes a 1.50 Square land and "h" denotes a hole size of 0.90 mm

s350 where "s" denotes a square SMT land size of 3.50 mm

r200_100 where "r" denotes a Rectangular SMT land 2.00 mm land length X 1.00 mm land width

b300_150 where "b" denotes a SMT Oblong land size of 3.00 mm X 1.50 mm

b400_200h100 where "b" denotes an Oblong land size of 4.00 mm length X 2.00 mm width and 1.00 mm hole

d300_150 where "d" denotes land with one circular end and one square end (looks like a D) 3.00 mm X 1.50 mm

v30h15l1-3 where "v" denotes a 0.30 mm blind via with 0.15 mm Hole; 1 is the starting layer, 3 is the end layer

r200_100r5 = Rounded Rectangular 2 mm X 1 mm X 0.05 mm radius corners

r200_100c10 = Chamfered Rectangular 2mm X 1 mm X 0.1 mm chamfered corners

v30h15l3-6 where "v" denotes a 0.30 mm buried via with 0.15 Hole; 3 is the starting layer, 6 is the end layer

These are the “Variants” or “Modifiers” that go after the basic padstack naming convention.

These are used when the User needs to change the padstack default values either by a different dimension or a different shape. In instances where shapes are different this becomes a two letter code with the modifier first followed by the land shape letter.

z = Inner Layer land dimension if different than the land on primary layer

x = Special modifier used alone or following other modifiers for lands on opposite side to primary layer land dimension

t = Thermal Relief; if different than IPC standard padstack – tid_od_sw for 4 spoke default

m = Solder Mask if different than default 1:1 scale of land

p = Solder Paste if different than default 1:1 scale of land

a = Assembly surface land if different than default 1:1 scale of land

y = Plane Clearance (Anti-pad) if the value is different than the Thermal OD

o = Offset Land Origin

k = Keep-out

r = Radius for Rounded Rectangular Land Shape

c = Chamfer for Chamfered Rectangular Land Shape

Shape change is the last letter in the string prior to the dimension.

USE of letter v: Vias can be named using the pad stack naming convention. Because most vias use lands that are circular in shape, the letter V will be used in place of the letter C in the padstack naming convention. If this is not true the modifiers can be added after the letter V to signify shape or dimensional changes to this default.

USE of letter w: In addition to Vias the padstack naming convention can also be used for defining mounting holes. The letter W shall be used to define the mounting hole characteristics and any associated lands used for the surface lands (either plated or un-plated).

Examples of double character modifiers:

ts = Thermal Square; if different than the top side land shape and dimensions

sw = Thermal spoke width

zs = Inner Layer Land Shape is Square (Note: The default is circular)

m0 = No Solder Mask

mxc = Solder Mask Opposite Side Circular

mx0 = Solder Mask Opposite Side No Solder Mask

xc = Opposite Side Circular

vs = Via with Square land

hn = Non-plated Hole

s150h90zs150 = where “s” is Square 1.50 land with 0.90 Hole with 1.50 inner (Z) Layer Square land

c150h90zc150 = where “c” is Circular 1.50 land with 0.90 Hole with 1.50 inner (Z) Layer Circular land

vs50h25 where “vs” denotes a 0.50 Square Via with a 0.25 Hole

v50h25xs70 where “v” is 0.50 Circular Via with 0.25 Hole and 0.70 Square land on opposite side

Order of precedence has been given to the first 4 modifiers.

Modifiers:

bl – bottom left

br – bottom right

ul – upper left

ur – upper right

ulr – upper left & right

blr – bottom left & right

ubl – upper and bottom left

ubr – upper and bottom right

r100_200rbl50 = rectangular land 1.00 x 2.00 with 0.50 radius for rounded corner in bottom left corner

r100_200rbr50 = rectangular land 1.00 x 2.00 with 0.50 radius for rounded corner in bottom right corner

r100_200rul50 = rectangular land 1.00 x 2.00 with 0.50 radius for rounded corner in upper left corner

r100_200rur50 = rectangular land 1.00 x 2.00 with 0.50 radius for rounded corner in upper right corner

r100_200cbl50 = rectangular land 1.00 x 2.00 with 0.50 chamfer for chamfer corner in bottom left corner

r100_200cbr50 = rectangular land 1.00 x 2.00 with 0.50 chamfer for chamfer corner in bottom right corne

r100_200cul50 = rectangular land 1.00 x 2.00 with 0.50 chamfer for chamfer corner in upper left corner

r100_200cur50 = rectangular land 1.00 x 2.00 with 0.50 chamfer for chamfer corner in upper right corner

Chamfered and Rounded Rectangular with all four corners chamfered does not need a corner modifier.

r200_100r50 = rectangular land 2.00 x 1.00 with 0.50 radius for rounded corners in all 4 corners

r200_100c50 = rectangular land 2.00 x 1.00 with 0.50 chamfer for chamfered corners in all 4 corners

c150h90 = Default padstack with a 1.50 circular land with a 0.90 hole (no modifiers used)

c150hn90 = Default padstack with a 1.50 circular land with a 0.90 non-plated hole (no modifiers used)

c150h90z140 = Inner layer land is smaller than external lands 1.40 or 0.10 smaller

c150h90z140x170 = Opposite side land is larger than top side land 1.70 or 0.20 larger

c150h90z140x170m165mx185 = Solder mask opening for top and bottom lands 0.15 larger for each

c150h90z140x170m165mX185a200 = Assembly drawing land in 0.50 larger than 1.50 primary land

c150h90z140x170m165mx185a200y300 = Plane clearance anti-pad diameter is 3.00

c150h90z140x170m165mx85 = Solder mask encroachment on opposite land by 0.65 smaller

c150h90m165 = adding a solder mask opening of 1.65 diameter or 0.15 larger than land

c150h90t150_180_40 = Thermal ID 1.50, OD 1.80, Spoke Width 0.40, Anti-pad 1.80

c150h90t150_180_40y200 = Anti-pad 2.00 (because the size is different than the Thermal OD)

c150h90t150_180_80_2 = Spoke Width 0.80 with 2 Spokes

c150h90m165t150_180_40 = Solder Mask 1.65

Sample – b = Oblong Land Shape then “X” dimension (length) then Underscore _ “Y” dimension (width)

b400_200h300_100 = Oblong land 4mm length X 2mm width with slotted hole size 3mm X 1mm

b400_200hn300_100 = Oblong land 4mm X 2mm with non-plated slotted hole size 3mm X 1mm

b300_150 = Default padstack with a 3.00 length and 1.50 width land (no modifiers used)

b300_150m330_180 = Solder Mask is 0.30 larger than the land

b300_150m330_180p240_140 = Solder Paste is smaller by 0.10 width and 0.60 length

b300_150b-50 = Oblong Land 3.0mm X 1.5mm w/Offset Origin negative 0.5mm

r400_200po430_230 = Rectangle SMT land 4.00 X 2.00 with a Oblong Solder Paste size of 4.30 X 2.30

Square Configurations

s480p4s152 = 4.80mm Square Land with 4 Paste Mask Squares 1.52mm each

s480p4s152cul50 = 4.80mm Square Land with 4 Paste Mask Squares 1.52mm each with 0.50mm Chamfer in Upper Left corner

s480p4s152cul50r25 = 4.80mm Square Land with 4 Paste Mask Squares 1.52mm each with 0.50mm Chamfer in Upper Left corner with 0.25mm corner Radius

w700h400z520m720 = This is a Plated Through Mounting hole for a #6-32 screw using a 4.00 diameter hole and having a circular 7.00 land on the primary and secondary side of the board, with a solder mask clearance that is 0.20 larger than the 7.20 land. The internal lands are smaller that the external and are also circular 5.20 in diameter.

w700hn400z520m720 = Non-plated version

c100m200k200 = Circular Land 1.00 with Solder Mask 2.00 with Keep-out 2.00

s100m200k200 = Square Land 1.00 with Solder Mask 2.00 with Keep-out 2.00

c150h100 = 1.5mm circular pad with 1mm hole with 1.5mm solder mask with 1.5mm plane clearance with 1.5mm assembly outline with Thermal Relief w/4 spokes 0.4mm width with ID 1.5mm and OD 1.8mm

c100h150 = 1mm circular pad with 1.5mm hole with 1.5mm solder mask with 2.35mm plane clearance with 2.1mm keep-out

Another example of padstyle of the top "layer 1" may be different to the inner and bottom layers is a TO-220 horizontal where you have a rectangular pad to connect with the heatsink of the device and have only a round pad on inner and the bottom layer.

r1599_1039r25o510xc580zc580h385 = rectangular 15.99 mm x 10.39 mm, radius 0.25 mm corners for a pad on layer 1, where the centre of the rectangular pad is off-set 5.1 mm from the centre of the hole. Hole size is 3.85 mm. Pads on inner layers and the bottom size is a round 5.80 mm.

typedef struct
{

to be added

} PadStack;