Footprints / Land Patterns - IPC-7352 strange evolutions

IPC-7352 strange evolutions

Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: Footprints / Land Patterns
Forum Description: [General or a CAD specific issues / discussions]
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=3576
Printed Date: 18 Nov 2025 at 2:51pm

Topic: IPC-7352 strange evolutions

Posted By: sot23
Subject: IPC-7352 strange evolutions
Date Posted: 18 Nov 2025 at 8:23am

Hello, my team recently purchased the IPC-7352 released in 2023 and I am currently in the process of studying it to decide whether we should make it our new standard for footprints creation or not.

For the moment I must admit that I am not thrilled by what I have read.

Some exemples :

Page 4 : Figure 3-2 depicts an SOIC instead of a 1206 capacitor. I know errors can happen, but on a document of this stature, it makes me question the review process if there is already that kind of mistake on page 4.
Page 10 we are introduced to the new method to calculate "Rectangular or square end components [...] where leads are 1, 2, 3 or 5 sided", the Toe calculation for such a component with a lead widths equal or larger than 0.5mm gives me abnormal results. It is said to be "25% of the nominal height of the component, or 0.5mm, whichever is less" for B level. If I take a very standard 0402 resistor from Vishay, TNPWe3 serie (width = 0.5 +/-0.05), with a nominal height of 0.35mm, it gives me a toe of 0.0875 (rounded to 0.09). That is less that the 0.15mm toe recommended for C level. How can that be possible ?
Round off factor for Chip components smaller in widths than 0.5mm is 0.005mm increments. Has this been discussed with a PCB manufacturer ? 5µm variation on a PCB geometry seems quite small... And it will give an absolutely crazy amount of variations for the same footprint depending on the small variations by component manufacturers.
Section 4.4.1 "Nominal Hole Diameter" describes a method for calculating drill hole diameter. It is different than the method used in IPC-2222. Which one should we use ? This method doesn't take the board level into account, and therefore, doesn't take the tolerance of the hole into account. Seems odd. For exemple, for a round terminal on a 1.6mm thick board, the hole should be "Terminal diameter max + 0.15mm". On a level A PCB with 0.2mm tolerance, assuming it is centered, it would leave only 0.05mm more that the terminal diameter max which does not seem enough.

My question : what do you all think about 7352 ?

I would be very interested in your opinion specifically, Tom H, as I know you are very much involved in the IPC talks (thanks for all your work on that by the way). Is it a good upgrade to 7351B ? Honestly I was hoping for more.

But maybe I am a bit to difficult...

Sorry if my English is not perfect, as it is not my primary language.

Replies:

Posted By: Tom H
Date Posted: 18 Nov 2025 at 8:56am

IPC-7351B and IPC-7352 are identical for Surface Mount. No change except the pad stack naming convention added a double 'rr' for Rounded Rectangle pad shape.

IPC-7352 introduced Through-hole technology, but most of the information was extracted from IPC-2221 & IPC-2222. The main thing that was added was the Through-hole land pattern naming convention which we created in 2008 but shelved until 2023.

The IPC-735x series misses the mark in several areas.

- Solder joint goals 'one size fits all' doesn't produce the best assembly attachment and it doesn't adhere to IPC J-STD-001. Also, the values between density levels is too robust. Most is too Most and Least is too Least.

- The naming convention puts the 'pin qty' at the end of the footprint name. This was changed in the IPC-7351C standard that was unanimously approved by the land pattern committee but never got released.

- The Zero Component Rotation differs from the standard they replaced - IPC-SM-782

https://www.pcblibraries.com/forum/ipc7352-vs-pcb-libraries-footprint-naming-option_topic3488_post13869.html?KW=IPC%2D7352#13869" rel="nofollow - https://www.pcblibraries.com/forum/ipc7352-vs-pcb-libraries-footprint-naming-option_topic3488_post13869.html?KW=IPC%2D7352#13869

https://www.pcblibraries.com/forum/pcb-pad-footprint-orientation_topic3460_post14010.html?KW=IPC%2D7351B#14010" rel="nofollow - https://www.pcblibraries.com/forum/pcb-pad-footprint-orientation_topic3460_post14010.html?KW=IPC%2D7351B#14010

-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - X - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn