Print Page | Close Window

Footprint Creation Strategy for Common Packages

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=3484
Printed Date: 19 Apr 2025 at 3:53pm


Topic: Footprint Creation Strategy for Common Packages
Posted By: giggio
Subject: Footprint Creation Strategy for Common Packages
Date Posted: 16 Apr 2025 at 2:06am
Hello everyone,

I'm new to PCB library creation and am currently facing some challenges in understanding the best practices for building footprints in Altium.

Specifically, I'm starting with a common package like SOT23 and am unsure about the criteria to use for creating a generic footprint that can be utilized for multiple part numbers.

From my research, it seems there isn't a universally recognized standard. JEDEC isn't universally adopted, and while IPC is often referenced, I haven't found a standard mechanical drawing for a typical SOT23 there. I could refer to a datasheet from a specific SOT23 chip manufacturer, but each manufacturer seems to have slightly different dimensions.

Furthermore, once I create this "standard/universal" SOT23 footprint, what criteria should I use to determine if it can be associated with a specific part number? Will the "standard/universal" SOT23 footprint always be suitable, or will I often need to create a new one? What tolerance values should I consider to decide if I can assign an existing footprint to a part number or if I must create a new one?

Following a discussion with an experienced PCB layout master, the focus of my concern is managing the slight dimensional differences found in datasheets for components with the same nominal package (e.g., SOT23-5) but from different manufacturers.

My specific questions, considering this discussion, are:

    Strategy for creating a "generic" footprint for a package like SOT23: Instead of relying on a single datasheet, what criteria should I follow to create a footprint that can accommodate most SOT23 components (e.g., by considering the maximum dimensions found across various manufacturers' datasheets)?
    Criteria for associating an existing footprint with a new part number: Once I have an SOT23 footprint in my library, how can I determine if it's appropriate to associate it with a new integrated circuit in an SOT23 package? What tolerance values should I consider when comparing the component dimensions in its datasheet to the dimensions of the existing footprint? Are there any guidelines (perhaps based on IPC or best practices) to establish if the differences are acceptable or if a new, specific footprint is necessary?
    Does it make sense to create manufacturer-specific footprints (e.g., SOT23-ST vs. SOT23-Texas Instruments)? What are your opinions on this approach, and what are the pros and cons?
    Library Guidelines: What general procedures or guidelines should I document for footprint management so that future library users know how to decide whether to use an existing footprint or create a new one, taking into account tolerances and dimensional variations?

I understand that experience plays a crucial role, but I'd like to define some objective procedures to ensure consistency in footprint creation and usage.

Thank you in advance for your help!


Replies:
Posted By: Tom H
Date Posted: 16 Apr 2025 at 9:12am
I think you need to download and install the Free "Footprint Expert Calculator" and open the "Surface Mount > SOT-23" component package family and see the different pin quantities. 

The 1987 EIA PDP-100 was the original standard for SOT-23 package dimensions, but that publication went obsolete 30 years ago. However, Global still sells it. 

The 1999 JEDEC TO-236 superseded the EIA PDP-100. 

However, no component manufacturers use the JEDEC dimensions. They all have different dimensions for package height, width, length, but the pin pitch is always 0.95 mm. 

The PCB Libraries footprint naming convention handles all the package variations. No need to include the manufacturers name in the footprint. 



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

Posted By: giggio
Date Posted: 16 Apr 2025 at 2:00pm
Thanks a lot Tom.

But what I like understand is where I can recovery "standard" footprint for more that can fit most of the SOT23-3 used by various manufacturers. 

I would like to have only one SOT23-3 and assign it to multiple P/Ns from different manufacturers.

This is an example for the SOT23-3 but the same goes for any other footprint.

Posted By: Tom H
Date Posted: 16 Apr 2025 at 3:18pm
Ah yes, the one master pattern that will accommodate multiple manufacturers packages. 

This is almost impossible using the IPC mathematical model that includes terminal tolerances for the pad stack calculation. However, if you gather all the package dimensions for all your sources and neutralize the tolerances by taking the high and low and figure out the average terminal lead tolerance. 

The package height has nothing to do with the footprint calculation, but it is used to create the 3D STEP model. 

The average nominal SOT-23 package dimensions:
  • Body length - 1.60 +/- 0.20
  • Body width - 0.80 +/- 0.10
  • Terminal Lead Span - 1.60 +/- 0.20
  • Lead Width - 0.225 +/- 0.075
  • Lead Length - 0.20 +/- 0.10
The final drafting outlines for the footprint will use the Maximum dimensions (Nominal + Tolerance). 

The pad size will be maximum terminal lead + Toe, Heel and Side goals. 

Footprint Expert is an excellent resource for calculating a standard pattern for all SOT-23 packages. You insert all the package dimensions for each vendor and save that data to an FPX file library. Then the footprint names contain the package dimensions. 

You can create an FPX file with SOT-23 package dimensions and the Physical Description will display all the dimensions. 

You can also select "Utilities > Find Duplicate Entries > Footprint Name" and your goal is to have the same footprint name in your FPX library. 

If you Batch Build all the SOT-23 library parts, Footprint Expert will only create one of them, as the CAD tool library can't handle duplicate footprint names. 

If you're knowledgeable about IPC J-STD-001 and solder joint goals, you can use the "Nominal Calculation Mode" calculator that does not require package tolerances (only nominal package dimensions) and create your own Toe, Heel and Side solder joint goals then you can create a master "One Size Fits All" pattern. 

We offer free unlimited technical support education for all Footprint Expert users. We not only teach the program features, but go into technical details on all the standards for land pattern calculation. 



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


Print Page | Close Window