PCB Libraries Forum Homepage
Forum Home Forum Home > PCB Footprint Expert > Questions & Answers
  New Posts New Posts RSS Feed - Footprint Name for Parts With Tabs
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

Footprint Name for Parts With Tabs

 Post Reply Post Reply
Author
Message
dipakdesai View Drop Down
New User
New User


Joined: 08 Aug 2012
Location: Frisco, Texas
Status: Offline
Points: 8
Post Options Post Options   Thanks (0) Thanks(0)   Quote dipakdesai Quote  Post ReplyReply Direct Link To This Post Topic: Footprint Name for Parts With Tabs
    Posted: 08 Aug 2012 at 8:56am
Hi
 
I would like to suggest to add the tab dimension in the footprint name for all parts with tabs example
 
QFN50P1000X1000X90-69N580EP so in this I have added the 5.8mm TAB in the name.
 
Also there are a lot of SOIC packages that have rectangular tab so in these cases it would be better to add 123x456EP. example SOIC127P780X200-14N095x120EP
 
I would be good to add the EP to identify the exposed pad (the TAB) also as shown in the example above.
 
Would it also be better to add a dash in between the N ans the tab dimension e.g SOIC127P780X200-14N-095x120EP
QFN50P1000X1000X90-69N-580EP
 
 
Thanks
Dipak Desai
 
Back to Top
Tom H View Drop Down
Admin Group
Admin Group
Avatar

Joined: 05 Jan 2012
Location: San Diego, CA
Status: Offline
Points: 5239
Post Options Post Options   Thanks (0) Thanks(0)   Quote Tom H Quote  Post ReplyReply Direct Link To This Post Posted: 21 Oct 2012 at 1:30pm

The IPC Land Pattern Subcommittee has approved the use of 3 modifiers at the end of Land Pattern names.

 

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.

 

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

 

There are 3 component features that affect the footprint name –

1.    Thermal Tab Size = SOP50P710X120-14NT300

·         T300 = 3.00 mm Square Thermal Pad

·         T300X200 = 3.00 mm X 2.00 mm Rectangle Thermal Pad

2.    Lead Length Tolerance = SOP50P710X120-14NL50

·         L50 = 0.50 mm Nominal Terminal Length

3.    Ball Size = BGA121C50P11X11_600X600X100NB23

·         B23 = 0.23 mm Nominal Ball Diameter

 

These would be used at the end of the Land Pattern Name only if a new Land Pattern is added to the user library with an identical Land Pattern Name but different T, L or B.

Example: Create a BGA chart that has a default Ball Size for each Pin Pitch.

Pin Pitch

Nominal Ball Diameter

1.50

0.90

1.27

0.75

1.00

0.60

0.80

0.50

0.75

0.45

0.65

0.40

0.50

0.30

0.40

0.25

0.35

0.22

0.30

0.20

 

 

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

Back to Top
 Post Reply Post Reply

Forum Jump Forum Permissions View Drop Down



This page was generated in 0.078 seconds.