PCB Libraries Forum Homepage
Forum Home Forum Home > Libraries > Footprints / Land Patterns > Altium
  New Posts New Posts RSS Feed - Max Pin Tolerance Exceeds Calculated Pad Size
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

Max Pin Tolerance Exceeds Calculated Pad Size
 Post Reply Post Reply
Author
Message
  Topic Search Topic Search  Topic Options Topic Options
Michael Ramonette View Drop Down
New User
New User


Joined: 13 Dec 2016
Status: Offline
Points: 4 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Michael Ramonette Quote  Post ReplyReply Direct Link To This Post Topic: Max Pin Tolerance Exceeds Calculated Pad Size
    Posted: 18 Aug 2023 at 10:19am
A nominal footprint that was created with the parts calculator with a pin max width of 0.35 mm and a minimum width of 0.30.  

The concern I have is the pad is calculated at 0.32 mm and if we get a batch of parts that are created at the max tolerance the pin will overhang the pad on the b measurement.  

Is this correct or am I missing something?  

What do I tell my Engineers?

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

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 18 Aug 2023 at 12:21pm
What version of Footprint Expert are you using? 

What is the component family of the footprint you're creating?
Stay connected - follow us! X - LinkedIn
Back to Top
Michael Ramonette View Drop Down
New User
New User


Joined: 13 Dec 2016
Status: Offline
Points: 4 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Michael Ramonette Quote  Post ReplyReply Direct Link To This Post Posted: 18 Aug 2023 at 2:36pm
16 pin QFN with pad 

I had my librarian re-create it with a newer version of library expert with the same results.

MAX8556ETE+
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 18 Aug 2023 at 2:55pm
The Side solder joint goal for the "Flat No-Lead (Side)" is set to -0.04. 

If this is troubling you and your engineers then do this. 

Go to "Tools > Options > Terminals > Surface Mount > Flat No-Lead (Side) > Side goal" and change the value from -0.04 to -0.02 and your pad width will recalculate to 0.36 mm

All the values in Footprint Expert are editable. If you don't like a value set forth in the IPC-7351B standard then change it. 

Here is the Flat No-Lead Table 3-15 in IPC-7351B (and an explanation of the negative solder joint goals: 


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


Joined: 13 Dec 2016
Status: Offline
Points: 4 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Michael Ramonette Quote  Post ReplyReply Direct Link To This Post Posted: 18 Aug 2023 at 4:28pm
Does this violate IPC-7351B or C?  

We have an IPC library and are contently questioned on parts created for one reason or another.  

If it does violate IPC suggestions I will be creating this as alternate part.

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

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 18 Aug 2023 at 4:59pm
IPC-7351C was canceled and replaced with IPC-7352 which includes through-hole technology. 

IPC-7352 is NOT a Standard. It's a Generic Guideline for Land Pattern Design. 

There's no such thing as violating a Guideline. A Guideline is a suggestion or recommendation. 

You mentioned that the default side solder joint goal for a Flat No-Lead QFN is 0.03 mm smaller than the maximum terminal lead width. 

Tell your engineers that you're adjusting the "Guideline" by less than 1 mil because you're paranoid that the pad width is too small. 

The main reason why the Guideline suggests a -0.04 mm side goal is because of the 0.40 mm pin pitch QFN where the pad sides would be too close together and violate your minimum pad to pad spacing. 

Also, you can't run a trace between a 0.50 mm pin pitch QFN. So the maximum lead hanging over the pad slightly won't affect anything. 
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: 21 Aug 2023 at 12:13pm
Dear Michael,

Which values are you using for fabrication/assembly tolerances in this case? 
The default values? 0.00 mm? 

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: 5718 		Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 21 Aug 2023 at 12:34pm
0.00 Fabrication & Assembly Tolerances are the new norm per IPC-7352. 

But all the negative solder joint goals are 0.00 too. 

There is an IPC-7352.opt file that updates all the options to do this. 

However, if you open the IPC-7352.opt file, don't forget to save it under a different name before you start editing it because it will be overwritten with a new installation. 
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 0.203 seconds.