Posts Tagged ‘Padstack’

3 June, 2011
IPC introduced a new padstack naming convention in the IPC-7351B standard publication and it is used exclusively in the Mentor Graphics LP calculator. This article explains the breakdown of the new standard and its benefits.

The padstack 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 (pad) shape. There are six basic land shape identifiers. Note: All alphabetical characters are “lower case”. This helps discriminate numeric values.

Basic Land Shape Letters –

  • c = Circular
  • s = Square
  • r = Rectangle
  • b = Oblong
  • d = D-shape (Square on one end and full radius on the other end)
  • u = User defined contour (Irregular shape)

 The “b” was used for Oblong because the letter “o” can easily be confused with the character zero “0”.

 The next section of the naming convention addresses assumed defaults. This is to keep the default padstack name short and simple. Any deviations from these padstack defaults require the use of special modifiers.

  • Solder Mask is 1:1 scale of the land size
  • Paste Mask is 1:1 scale of the land size
  • The Assembly Layer land is 1:1 scale of the land size

  • Inner Layer Land is the same shape as the outer layer land

  • The Primary and Secondary lands are the same size

  • The inner layer land shapes are Circular

  • Vias are Circular

  • Thermal ID, OD and Spoke Width sizes follow the IPC Level A, B or C

  • Thermal Reliefs have 4 spokes

  • Plane Clearance Anti-pad size follows the IPC Level A, B or C

  • Mounting Holes are Circular

 Every board fabricator’s ability to register solder mask is different. The 1:1 scale solder mask default compensates for the variation, and so long as manufacturers are building to standard specifications such as the IPC-6012 that states you can’t have miss-registration of the solder mask. It’s important that when you are creating a CAD library that will be used for various trace/space combinations, that you leave the responsibility of the solder mask swell up to the fabrication CAM operator when they are panelizing your Gerber or ODB++ data. By having all of the solder mask sizes 1:1 scale of the land (pad) size, you are providing the manufacturer with a known starting point for them to work with.

I need to explain an exception to this rule for creating solder mask defined lands for BGA’s. IPC does not recommend solder mask defined BGA CAD library parts but some companies use this technique for very fine pitch parts that require a small diameter land size. In this case, the solder mask acts as an adhesive to secure the land to the PCB Prepreg to withstand drop testing for hand held electronic products. It has been proven in drop tests for hand held electronic devices that a fine pitch BGA solder joint is more secure than the land attachment to the Prepreg. i.e.: during drop testing, a fine pitch BGA pad will rip away from the PCB Prepreg material before the BGA solder joint fails. See the picture on the right side in Figure 1 as an example of a solder mask defined BGA land.   

Figure 1 - Solder Mask Defined BGA Land

Figure 1 - Solder Mask Defined BGA Land

 

 Solder mask defined lands are also used for Flexible circuit boards for the same reason, to hold the land (pad) to the PCB surface to prevent the land from ripping away from the PCB material. When you use solder mask defined lands you must indicate which parts deviate from the 1:1 scale solder mask rule in the fabrication drawing notes to notify the CAM operator not to swell these solder mask features.

 In the padstack naming convention there are illegal characters that should never be used. These include “ ” , ; : / \ [ ] ( ) . { } * & % # $ ! @ ^ =

 Examples utilizing the “Basic Land Shape Letters” (all padstack values are in metric units)

 Note: Every number goes two places to the right and as many places 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

c150h90 - where “c” denotes a Circular land with a 1.50 diameter and H denotes a hole size of 0.90

v50h25 – where a “v” denotes a via with a 0.50 land (default Circular land) and H denotes a 0.25 hole

s150h90 – where “s” denotes a 1.50 Square land and H denotes a hole size of 0.90

s350 – where ‘s” denotes a square SMT land size of 3.50

r200_100 – where “r” denotes a Rectangular SMT land 2.00 land length X 1.00 land width

b300_150 – where “b” denotes a SMT Oblong land size of 3.00 X 1.50

b400_200h100 – where “b” denotes an Oblong land size of 4.00 length X 2.00 width and 1.00 hole

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

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

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

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

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

  Special modifiers are used when padstack features are different than the defaults. 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.

 

These are single letter modifiers –

n = Non-plated Hole

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

 

These are double letter 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

 

 Land shape change is the last letter in the string prior to the dimension.

 Examples of single letter modifiers with a Circular Plated Through-hole land –

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

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

 

 Examples of single letter modifiers for an Oblong Surface Mount land –

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

 

 Examples of a padstack with Oblong land with Slotted Hole –

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

 

 Chamfered & Rounded corner modifiers are used to indicate which corner(s) are modified.

 See figure 2 for the “order of precedence” that has been given to the first 4 modifiers.

Figure 2 - Chamfered Land Variations

Figure 2 - Chamfered Land Variations

 

 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

 Rounded and Chamfered lands in “one corner” Modifier Examples:

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 corner

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.

Modifier Examples with Rounded Rectangle Land Shape: 

Rounded Rectangular Land Shape

Rounded Rectangular Land Shape

r200_100culr50 = rectangular land 2.00 x 1.00 with 0.50 chamfer for chamfered corners in 2 corners

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

 

Modifier Examples with Chamfered Rectangle Land Shape: 

Chamfered Rectangular Land Shape

Chamfered Rectangular Land Shape

r100_200r50 = rectangular land 1.00 x 2.00 with 0.50 radius for rounded corners in all 4 corners

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

 

 Thermal pads can have a combination of chamfered and rounded corners however the typical application is 2 variations. The most prominent is a chamfered corner located near pin 1 and the second is a chamfered corner located near pin 1 with the other 3 corners rounded. These two variations are the default.

Square Configurations

Thermal Pad with 4 Square Corners

Thermal Pad with 4 Square Corners

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

Thermal Pad with Chamfered Corner

Thermal Pad with Chamfered Corner

u480p4s152cul50 = 4.80mm Square Land with 4 Paste Mask Squares 1.52mm each with 0.50mm Chamfer in Upper Left corner

Thermal Pad With Chamfered Corner Rounded Corners

Thermal Pad With Chamfered Corner Rounded Corners

u480p4s152cul50r25 = 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

 

 Example of a Local Fiducial for Fine Pitch SMT Components:

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

See Figure 3 for Local Fiducial application used for fine pitch components.  

Figure 3 - Local Fiducials

Figure 3 - Local Fiducials

 

 Did you know that you can download a free 10-day trial license for LP Wizard here – http://www.mentor.com/go/lpwizard

 After the 10-day trial license ends, the LP Wizard will run in “Demo Mode” as an IPC-7351B LP Calculator. The LP Calculator auto-generates padstack names using the convention mentioned in this article.  

, , ,

31 March, 2011

Here are some tips about Metric Speak that all PCB designers need to know. “Metric” is not a unit of measure. Metric is a term that describes a measurement system. You use either millimeters or microns for your PCB design units. The proper terminology to describe your working units when using the metric measurement system is millimeters or microns, not metric. Example: When doing PCB layout in Inches or Mils you never refer to working in “Imperial Units”.

Millimeters allow finer (and greater) granularity in the PCB design grid system to optimize board real-estate, part placement, via fanout and routing trace/space features and snap grids. This will be very important in the future of PCB RF Micro-technology. PCB impedance measurements are more accurate in Micron units than “Ounces of Copper” and Mil core/Prepreg dielectric. Use Micron Units to achieve the highest level of accuracy for impedance calculations.

Unfortunately, PCB manufacturers are directly responsible for holding back the progress of the transition to metrication of our industry. When the PCB fabrication companies transitions to the metric system, the entire electronics industry will achieve the peak of “electronic product development automation”. Until then, we’ll plod along using dual units in the land of chaos.

Here is an example of the chaos in the Chip Component family. All Chip names refer to their body length and width. When EIAJ introduced the standard Chip and Molded body component dimensions, only millimeter units were used. A 3216 was 3.2 mm long and 1.6 mm wide. It was very simple. When the data was passed on to EIA in America, they changed all the chip names from millimeters to Inches and a 3216 was renamed 1206 or 0.125” length and 0.062” width (just drop the 3rd place number). Today most component manufacturers dimension all there component packages in millimeters see Table 1 that illustrates Metric vs. Imperial names. You can easily see the confusion in the dual measurement system.

Table 1 - Chip Component Names

Table 1 - Chip Component Names

Let’s start the transition process. 99% of all PCB layouts use vias. See Table 2 for an Inch to Millimeter chart for common via sizes starting with a 0.15 mm hole and growing in 0.05 mm increments. I’ll provide the entire padstack conversion. I intentionally did not add thermal relief data because vias should have a direct plane connection (no thermal relief is necessary). When transitioning from Imperial units to Metric units, always round-off the millimeter values in 0.05mm increments for normal resolution. If you’re working on extremely dense hand held device technology, round-off to the nearest 0.01 mm. For PCB design, there is no reason to go more than 2 places to the right of the decimal point for the present. 0.01 mm = 0.0003937”

Table 2 - Via Padstack Technology

Table 2 - Via Padstack Technology

 Table 3 illustrates 4 common inch based part placement grids and their millimeter equivalent.  The common rule in placing parts in millimeters is to always stay one place to the right of the decimal or 0.1 mm increments.

Table 3 - Component Placement

Table 3 - Component Placement

 Table 4 provides all the common trace/space technology and routing snap grids. The common rule when working in millimeters is to always use a 0.05 mm routing grid. Most component lead pin pitches are 0.05 mm increments and IPC-7351B land (pad) sizes and snap grids are in 0.05 mm increments. This totally optimizes trace routing and eliminates wasted PCB real-estate. Everything fits together tighter than Lego building blocks.  Notice that in the inch units, a gridless shape-based option is used, but in millimeters all objects can easily snap to a grid and still achieve maximum density solutions. I provide 3 various route snap grid solutions for the various trace/space rules.

Note: Inch based routing grids are evenly divisible into 0.100” while millimeter based routing grids are evenly divisible into 1 mm.

Table 4 - Trace Widths & Optimum Routing Grids

Table 4 - Trace Widths & Optimum Routing Grids

 Table 5 provides the PCB material equivalents. Note that the various columns are not related to each other. Each column describes a specific PCB feature. In the first column “Board Thickness” is common PCB finished material thicknesses and the metric equivalent rounded off to the nearest 0.1 mm. The second column is copper weight in ounces and their micron equivalent. Using microns to describe copper thickness is better than using weight. The third and forth columns go together. Column 3 defines the type of hole and column 4 provides the PCB fabrication tolerance for each different hole type in the chart.

Table 5 - PC Board Criteria

Table 5 - PC Board Criteria

 Table 6 is common plated through-hole padstacks for component leads and their inch to millimeter conversion. All hole, pad and plane clearance values are in 0.05mm increments. The Solder Mask is the same value as the outer layer pads. This padstack information was taken from the proportional padstack table and you can download it here under “Appnote 10836: Proportional Through-hole Padstacks” – http://www.mentor.com/products/pcb-system-design/library-tools/lp-wizard/import-docs

Note: this downloadable chart only contains millimeter values and not the inch equivalents in Table 6.

Table 6 - Common Plated Through-hole Padstacks

Table 6 - Common Plated Through-hole Padstacks

 Table 7 is common non-plated through-hole padstacks and their inch to millimeter conversion. All hole, pad and plane clearance values are in 0.05mm increments. The Solder Mask is the same value as the hole size to allow the PCB manufacturer to oversize it per their specific fabrication tolerances. Notice that the pad size for every padstack is 1.00 mm. Because the holes are not plated, the hole size is typically larger than the hole size. Also, there is no reason to have multiple pad sizes when the pad is eventually drilled away. The only reason for having a pad in a non-plated padstack is display a marker as a guide for the hole location. The PCB manufacturer does not need the pad in the padstack, but sometimes when there is no pad (but there is a drill hole) the manufacturer might question if the hole is valid. Of course there is no thermal relief required in non-plated hole padstacks.

Table 7 - Common Non-Plated Through-hole Padstacks

Table 7 - Common Non-Plated Through-hole Padstacks

I want to note that the LP Calculator automatically performs all of these through-hole padstack calculations for you and provides 5 different options –

  1. Proportional Environment
  2. IPC-7251 Most Environment
  3. IPC-7251 Nominal Environment
  4. IPC-7251 Least Environment
  5. User Defined Environment Rules 

You can get a free LP Calculator by signing up for a 10-day evaluation of LP Wizard here – http://www.mentor.com/products/pcb-system-design/library-tools/lp-wizard/lp-wizard-eval

After the LP Wizard 10-day evaluation is over, the LP Wizard program will run in “Demo Mode” as LP Calculator.

, , ,

@MentorPCB tweets

  • Register for the upcoming U2U Automotive Conference in Detroit on Sept 10th! http://t.co/N198quxV3B
  • Charles talks about an upcoming event: Learn more about the new release of Xpedition - http://t.co/2Y0juFAESY
  • Look out for upcoming events. Charles will give you all the insight. Learn more about the new release of Xpedition - http://t.co/2Y0juFAESY

Follow MentorPCB