Questions & Answers - Too many SOT 23s

Too many SOT 23s

Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: https://www.PCBLibraries.com/forum/forum_posts.asp?TID=651
Printed Date: 19 Nov 2024 at 7:16am

Topic: Too many SOT 23s

Posted By: DaveCowl
Subject: Too many SOT 23s
Date Posted: 30 Oct 2012 at 7:17pm

I am sure that this has been answered before but I can't seem to find it.

I have run up against two (only 2?) different SOT23-6 footprints (currently Maxim vs TI) with the same height and such so that the names of the library entries are the same.

FPX seems to keep both of them there... but what is going to happen if I do a mass export of land patterns?

It looks like I can manually edit the Footprint Name, so perhaps that is the place to start?

What is the accepted norm for naming (I recall A, B, etc. has fallen out of favour...).

Cheers!

Replies:

Posted By: Tom H
Date Posted: 30 Oct 2012 at 7:22pm

The object is to use the FPE FPX as a resource to Copy/Paste into you personal FPX. Your Company FPX should only contain parts your company uses.

Posted By: DaveCowl
Date Posted: 31 Oct 2012 at 9:39am

I understand that - both of these parts are on the same board.

Essentially the same part, just with quite different tolerances and pin dimensions for 'b' and 'L'.

Posted By: Tom H
Date Posted: 31 Oct 2012 at 10:08am

The variances in "b" and "L" will generate a different pad size and spacing. But the component Maximum Height value are different and that differentiates the footprint name.

Posted By: DaveCowl
Date Posted: 31 Oct 2012 at 11:32am

Actually the maximum height are identical. Hence the problem with naming...

I guess I could change one to be 0.01 mm different, which would result in a different name...

Posted By: Tom H
Date Posted: 31 Oct 2012 at 11:51am

IPC-7351C will recommend the following -

n The original IPC-7351 footprint naming convention does not include component tolerances, thermal pad sizes, BGA Ball sizes or various pin assignments into account. Therefore, the same component with different tolerances can produce a different land size and spacing with the same footprint name.

n A footprint name of SOP50P710X120-14N can have version A, B, C, D which do not indicate the variances.

n As you add parts to your library and you encounter a duplicate footprint name due to Thermal Pad size, Terminal Length Tolerance or Ball Size

1. Thermal Tab Size = SOP50P710X120-14NT300

· T300 = Thermal Pad 3.00 mm

2. Lead Length Tolerance = SOP50P710X120-14NL50

· L50 = Lead Length = 0.50 mm

3. Ball Size = BGA121C50P11X11_600X600X100NB23

· B23 = Ball Diameter 0.23 mm

n For component mfr. recommended footprint drop the environment level character after the pin qty. - SOP50P710X120-14

Posted By: DaveCowl
Date Posted: 31 Oct 2012 at 12:20pm

Ok great thanks.

The 'L50' type of option to define lead length should be adequate to differentiate the two.

Cheers!