Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

land pattern or foot print

Status
Not open for further replies.
soodamanikannan

soodamanikannan

Member level 5
Member level 5
Joined
Jul 16, 2010
Messages
82
Helped
4
Reputation
8
Reaction score
4
Trophy points
1,288
Location
Coimbatore
Activity points
1,704
Hi frnds,


Can we use data sheets land pattern size and hole size during foot print creation. Please give the confirmation. If its not correct please give the guideness to me. How to do as per standrad spec.
 

yes you should give the land pattern size as per the data sheet..because you are going to place the same ic to your board.
 
landpatterns dimensions and naming conventions are defined in IPC-7351. Datasheet landpatterns are different from IPC-7351 in a lot of cases.
 

If are going with IPC -7351 stranded always means go with the stranded.. some time we have to go with as per the data sheet..because the stranded will not match for your data sheet..if are able to impliment some of the things means you can impliment like text size of reference designator.pin numbering. pin one marking solder mask area and all..
 

IPC-7351 covers any footprint you want to create, what IPC-7351 does is set up the tolerences and pad sizes required for heal, to and side solder fillets etc, placement courtyards, also the naming format for both the footprint but also the padstack. If you buy the IPC-7351 spec you get a copy of the calculator, worth the money.
 

HI marce,

I referred the IPC 7351 STD. Stll we have some doubts. if i create the land pattern as per data sheet.

Example i had 10mil dia lead for a component during this condition how to choose the drill size and pad size.

And also i created the SMD device foot print for 0402 land.

Provided the mask clearence 5mil for all sides its fine or not.


Thanks in advance.
 

PTH holes add 0.1mm to diameter as a rule of thumb.
Pads for solder mask layer should be 1:1 with the following paragraph in you PCB manufacturing instructions:
3.11 Solder Resist
Solder resist (solder mask) is required on both external faces of the printed board, it shall meet the qualification/conformance IPC-SM-840 class H. Coverage, cure and adhesion shall be as defined in paragraphs 3.8.1 to 3.8.3 of IPC-6012, except that no encroachment of solder resist is allowed on any surface mount or ball grid lands, and that ALL pad patterns have solder resist slivers between individual pads. The height of the solder resist should not cause any mounting problems for surface mount components.
Solder resist data is provided as per IPC-7351 standard, 1:1 with the land size, the manufacturer is to oversize these solder resist openings commensurate with their manufacturing procedures ensuring that ALL the above requirements are met, the amount of oversize to take into account the minimum track and gap dimensions as shown on the Printed Boards Master Drawing. Solder resist not related to a component pad is not to be enlarged.

Do not size solder mask in your padstack otherwise you limit your design possibilities.
 

Oh I forgot, I'd use metric, most component these days are hard metric, and it makes life easier when you collaborate with mechanic design depts. and software.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top