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 Page  12>
Author
Message Reverse Sort Order
  Topic Search Topic Search  Topic Options Topic Options
Nick B View Drop Down
Admin Group
Admin Group


Joined: 02 Jan 2012
Status: Offline
Points: 1956 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Nick B Quote  Post ReplyReply Direct Link To This Post Topic: IPC-7351 and SMD Pad Shapes
    Posted: 24 Sep 2024 at 12:36am
Well said, quality and consistency is what it's all about.
Stay connected - follow us! X - LinkedIn
Back to Top
Back to Top
WilliamsimC View Drop Down
New User
New User


Joined: 19 Apr 2024
Status: Offline
Points: 14 		Post Options Post Options   Thanks (1) Thanks(1)   Quote WilliamsimC Quote  Post ReplyReply Direct Link To This Post Posted: 24 Sep 2024 at 12:18am
Hi Susan,

In my opinion, PCB Libraries chose to make the IPC-7352 approach an option instead of the default for a few key reasons. One important factor is library consistency. They want to ensure that users are fully aware of the changes and understand the implications of opting into the IPC-7352 approach. By not imposing this change on everyone, they help prevent any confusion or errors that might arise if users aren’t prepared for the differences.

Additionally, allowing users to choose the IPC-7352 option gives them flexibility. Some users may have established workflows or preferences that work well for them, and it’s important to respect that. This way, users can transition to the new approach at their own pace, ensuring they’re comfortable with it before making the switch. Overall, it’s about providing choices while maintaining clarity and consistency in the library.


Thanks,

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

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5788 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 19 Sep 2024 at 1:53pm
IPC-7351B adds Fabrication and Assembly Tolerances to calculate the resulting pad stack.

IPC-7352 removes the Fabrication and Assembly Tolerances for pad stack calculations. 

PCB Libraries (IPC-7351C) is only the Footprint Naming Convention. 

The typical package dimensions for a 1206 footprint are:
  • Length = 3.20 +/- 0.20
  • Width = 1.60 +/- 0.20
  • Terminal Lead = 0.50 +/- 0.25
The package dimensions and tolerances calculate the pad stack size and spacing.
Stay connected - follow us! X - LinkedIn
Back to Top
bab27 View Drop Down
New User
New User


Joined: 01 Sep 2024
Status: Offline
Points: 13 		Post Options Post Options   Thanks (0) Thanks(0)   Quote bab27 Quote  Post ReplyReply Direct Link To This Post Posted: 03 Sep 2024 at 11:30pm
Hello,

What are the main difference between IPC7351B and 7352 for land pattern dimension? 
Does IPC7351B use the tolerance RMS value like IPC7352 ?

It could be interesting to have a standard footprint size 1206 with nominal size (_N) and tolerance and the associated footprint calculation with the IPC7351B, 7352 and PCBlibrairies.

Thank you.
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5788 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 31 Jul 2024 at 10:44am
The Default is IPC-7351C (which was never released primarily due to Dieter Bergman's passing). 

The IPC 1-13 Land Pattern Committee worked on 7351C for 6 years and approved the new IPC J-STD-001 solder joint goals and the updated Naming Convention. 

We had to remove references to IPC-7351C and replace it as PCB Libraries. 

However, we do support IPC-7351B and IPC-7352 Options. 

We do not default to 7351B or 7352 because the solder joint goal tables do not compare with the recommendations from IPC J-STD-001 (but IPC-7351C did). 

However, Footprint Expert does default to the mathematical model for pad stack calculations for pad size and placement. This model takes into consideration the min/max tolerances of the component package terminal leads from the mfr. datasheet. 

The downside of using the terminal tolerances is that they are sometimes too robust and not realistic. And if you study the mfr. recommended patterns from millions of datasheets, they don't use the min/max terminal tolerances. They use the Nominal package dimensions. 

So even though IPC went to great lengths to create this mathematical model - uploads/3/IPC-7352_Mathematical_Model.zip

Component manufacturers do not use it for their recommended patterns displayed in their datasheets. 
Stay connected - follow us! X - LinkedIn
Back to Top
pcb0123 View Drop Down
New User
New User


Joined: 03 Jan 2013
Status: Offline
Points: 1 		Post Options Post Options   Thanks (0) Thanks(0)   Quote pcb0123 Quote  Post ReplyReply Direct Link To This Post Posted: 31 Jul 2024 at 9:12am
Hi Tom,
We are curious, what are the factors that have led PCB Libraries to make the IPC-7352 approach an option, rather than the default? Is library consistency the main driver, where you don't want to impose the change on users (where it might slip past their attention) and you want the user to be fully aware they are opting in to the newer IPC-7352 approach? Other reason(s)?
Thanks,
Susan
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5788 		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
dramos View Drop Down
Advanced User
Advanced User


Joined: 18 Feb 2021
Status: Offline
Points: 64 		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: 5788 		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: 64 		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
 Post Reply Post Reply Page  12>

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.250 seconds.