PCB Libraries Forum Homepage
Forum Home Forum Home > Libraries > Footprints / Land Patterns
  New Posts New Posts RSS Feed - IPC-7351 and SMD Pad Shapes
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

IPC-7351 and SMD Pad Shapes

 Post Reply Post Reply
Author
Message
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5645
Post Options Post Options   Thanks (1) Thanks(1)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Topic: IPC-7351 and SMD Pad Shapes
    Posted: 30 Dec 2019 at 2:51pm

IPC-7351B recommends an Oblong (or “Full Radius”) pad shape:



The component manufacturer’s recommend Rectangle pad shape:



PCB Libraries, Inc. recommends a Rounded Rectangular pad shape:



Paste mask stencil apertures are laser cut with rounded corners. It makes sense that the pad shape and stencil opening be the same.



I heard of a marketing slogan that mentioned “Rounded Rectangular pad shape is better for Lead-Free Solder”. This is not true. All pad shapes are good with Lead-Free Solder. A better statement would say “Rounded Rectangular pad shape is best. Period”.

Rounded Rectangle pad shapes were first introduced by the P-CAD software program 15 years ago. Then every other CAD vendor came out with their version of the Rounded Rectangular pad shape. The industry could not make Rounded Rectangular pad shape a standard or even a recommendation until all CAD tools supported it.

You can see that there is no solder in the rectangular pad shape corners. The question is “Why use Rectangular pad shape if there is no solder in the pad corners?”.

The post reflow oven results for Lead Solder on the left and Lead-Free Solder on the right.



In the Library Expert software program, the user has 100% control of the pad shape for every component family. You also control the percentage of the pad width to auto-generate the corner radius. You can also control the Maximum radius.

However, there are some component families that are “Bottom Only” terminal leads with square or rectangular shape. The pad size is a simple periphery around the terminal lead. These component families include DFN, LGA and PQFN with rectangle leads and the resulting pad shape should also be rectangular. Note: many DFN packages are less than 2.00 mm long and the pad size is 0.50 X 0.65 mm. Very small pad and the pad shape needs to be the same as the terminal lead shape for the best solder result as the pad and terminal lead size are 1:1 (same size).



The D-Shape pad is becoming popular, but not all CAD tools natively support this pad shape. As a result, the D-Shape pad is created from a copper poly shape. This makes the library part file size much larger, depending on how many pins are in the package. This translates to the PCB Layout file being larger too.

Stay connected - follow us! X - LinkedIn
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5645
Post Options Post Options   Thanks (1) Thanks(1)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 18 Dec 2023 at 6:19pm
Component packages are getting smaller and rectangular flat terminal leads are becoming popular. Flat square terminal leads like the Land Grid Array only require a 0.05 periphery to calculate the footprint. A 0.20 corner radius pad shape might expose the terminal lead. The terminal leads should always be on top of a pad and never be exposed outside a pad. 

There is no industry recommendations for the corner radius limit and no component manufacturers (except Texas Instruments) provide any guidance for the corner radius. 

A recommended pattern is provided in every new Texas Instruments datasheet and every recommended pattern has rounded rectangle pad shape with a corner radius of 0.05 mm. 

0.05 mm is the same radius as the paste mask stencil aperture opening cut by laser. 

I wish there was more guidance from assembly shops or the IPC J-STD-001 Standard, IPC-7093A, IPC-7351B or IPC-7352 regarding rounded rectangle pad shape corner radius limit, but it seems that the only industry documentation on this subject comes from Texas Instruments. 

Normally, a corner radius setting in a CAD tool is global to all footprint patterns. When the setting is 25% of the pad width, larger pads will have a huge corner radius and might expose the terminal lead. 

Whatever corner radius percentage and radius limit you choose to use is a personal setting for your PCB library. 

In the V24 Footprint Expert, the corner radius limit is set to 0.10 mm but users can change the value to whatever they want. 

Stay connected - follow us! X - LinkedIn
Back to Top
Frank_81 View Drop Down
New User
New User


Joined: 05 Jan 2024
Status: Offline
Points: 2
Post Options Post Options   Thanks (0) Thanks(0)   Quote Frank_81 Quote  Post ReplyReply Direct Link To This Post Posted: 05 Jan 2024 at 2:12pm
There is no industry recommendations for the corner radius limit and no component manufacturers (except Texas Instruments) provide any guidance for the corner radius. 

Hi Tom - Can you share the TI document name please? Is it available online? 

Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5645
Post Options Post Options   Thanks (1) Thanks(1)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 05 Jan 2024 at 3:02pm
Texas Instruments does not have a specific document for pad shape and corner rounding. 

Every TI datasheet has a "Mfr. Recommended Pattern" and the pad shapes are all rounded rectangle with a 0.05 mm radius. 


 

 
I'm seeing more and more manufacturer's recommending rounded corners. 

Here's a recommended pattern from Bourns.

  

 

Stay connected - follow us! X - LinkedIn
Back to Top
Frank_81 View Drop Down
New User
New User


Joined: 05 Jan 2024
Status: Offline
Points: 2
Post Options Post Options   Thanks (0) Thanks(0)   Quote Frank_81 Quote  Post ReplyReply Direct Link To This Post Posted: 05 Jan 2024 at 3:35pm
Thanks Tom for the detailed response. Appreciate you taking time to respond with details. 
Back to Top
dramos View Drop Down
Advanced User
Advanced User


Joined: 18 Feb 2021
Status: Offline
Points: 61
Post Options Post Options   Thanks (0) Thanks(0)   Quote dramos Quote  Post ReplyReply Direct Link To This Post Posted: 05 Mar 2024 at 7:52am
Dear Tom,

I have a question around this topic. 

PCBLibraries started with a Corner Radius size of 25% with a limit of 0.25mm and the new release has a limit of 0.10mm. 

I see it as an evolution. Besides, It is in the same way that the recommendation of some Manufacturers.

My question is, what you have seen to make this evolution? What you have detected on the new components/footprints to modify this value? Which is the main reason for this change?

As ever, thanks a lot for your comments.

Regards,
dramos
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5645
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 05 Mar 2024 at 9:55am
The corner radius was set to 25% of the pad width with a limit of 0.25 maximum radius. 

After building thousands of footprints for Parts on Demand (POD), we noticed every Texas Instruments recommended pattern had a 0.05 corner radius. 

We also noticed that the new mathematical model for IPC-7352 that turned off the fabrication and assembly tolerance calculated some pads to be slightly smaller (depending on the terminal tolerance). Also, there is an explosion of microminiature packages where the 0.25 corner rounding exposed package terminal leads. The metal component terminals were too close to the pad corners. 

You go through trial and error and test things out, but the end goal is to be safe and ensure that all terminal leads have full contact with the pad and consistent quality where all rounded corners are the same size. You get the best overall functionality with symmetrical cosmetically. 

PCB design is an art and the goal is to create beautiful yet functional PCB Layouts, 

It's also good for paste mask stencils where the aperture matches the pad shape. 

However, the setting is User Definable to allow you to change the default setting to whatever you want. 

Stay connected - follow us! X - LinkedIn
Back to Top
dramos View Drop Down
Advanced User
Advanced User


Joined: 18 Feb 2021
Status: Offline
Points: 61
Post Options Post Options   Thanks (0) Thanks(0)   Quote dramos Quote  Post ReplyReply Direct Link To This Post Posted: 06 Mar 2024 at 2:11am
Dear Tom,

Many thanks for your comments.

Yes, the PCB designers are little painters, sculptors (jejeje)

As the new IPC-7352 was downgraded to a guideline and we do not read anything strange about it in internet, we do not have bought it, but, is there a new mathematical model? 
I thought that was the same that we used in IPC-7351B, but with the recommendation of using for fabrication and placement tolerances 0.00 mm. (this is another topic that we will discuss another day)
and we should change the negative values of our solder Joints to 0.00mm as well. Am I in a error?

Best regards,
david

Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5645
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 06 Mar 2024 at 9:59am
Those 2 things were major updates in IPC-7352. 
  1. Fabrication and Assembly Tolerances changed to 0.00
  2. All negative solder joint goals changed to 0.00
The Fabrication tolerance was originally created in the 1980's to compensate for the etching process. But we all know this was unnecessary because all fabrication shops swell the outer layer features to compensate for their etching process tolerance. Appling a fabrication tolerance on a pad stack calculation and having the fabrication shop swell the outer layers is called a "Double Tolerance". It took IPC 40 years to figure that out. 

The Assembly tolerance was also created in the 1980's when pick and place machines required a tolerance of 1 mil (0.025). But the pick and place machine accuracy in 2024 is 0.01 mm and it might as well be 0.00 due to the 0201 chip package. Machines used in PCB Assembly and used to manufacture components are much more accurate today than 40 years ago. 

Stay connected - follow us! X - LinkedIn
Back to Top
 Post Reply Post Reply

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.078 seconds.