PQFN/PSON Footprint Name
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=305
Printed Date: 19 Nov 2024 at 7:36am
Topic: PQFN/PSON Footprint Name
Posted By: JZsori
Subject: PQFN/PSON Footprint Name
Date Posted: 01 Jun 2012 at 7:05pm
| There are multiple instances with the same name and description (PSON50P400X400X80-14, for example) but one has rectangular pads and the other has D-Shape pads. There should be some way to differentiate. |
Replies:
Posted By: Tom H
Date Posted: 22 Oct 2012 at 10:39am
|
The Component Lead Shape and the resulting Pad Shape have nothing to do with the footprint pattern name. Here is a component manufacturer that produces QFN packages with D-shape Package Leads -
Here is their recommended footprint with Rectangular footprint pads. Also notice that the Component Thermal Tab has a Chamfer Corner by Pin 1 and rounded corners on the others, but the manufacturer recommends a solid square with no chamfer or rounded corners. So it's really a "User Option". Also note that the manufacturer is calling the footprint a "Land Pattern" and they are using the IPC-7351 Land Pattern Naming Convention with the JEDEC variation in the Land Pattern Name (W6) to discriminate the Thermal Pad size. |
Posted By: Sanand
Date Posted: 27 Oct 2012 at 2:01am
|
Hi, I am new user for this site. I have some questions regarding the land pattern and wonder if this forum is suit for it. Do you know of any minimum clearance along the edge of PCB or memory module must be? Is it 0.050" to be minimum or 0.150"? And minimum gap between to components footprint or between two terminals of passive 0201? Thanks |
Posted By: Tom H
Date Posted: 27 Oct 2012 at 8:02am
|
The minimum board edge to any feature - component, via, trace, copper pour is 40 mils (1.0 mm). The minimum SMT component to component body or component pad to component pad gap is 10 mil (0.25 mm) for different components. The minumum pad to pad gap on the same component is 6 mils (0.15 mm). The minimum pad to thermal pad gap on the same component is 8 mils (0.20 mm). You can also get more information by reading my blog here - http://blogs.mentor.com/tom-hausherr/" rel="nofollow - http://blogs.mentor.com/tom-hausherr/ Copy/Paste the entire Blog into a Word document or print it out to PDF. We don't know how long Mentor Graphics will keep it available. |
Posted By: rdl86626
Date Posted: 29 Oct 2012 at 8:35am
|
Tom, I was reading the form where you stated “The minimum board edge to any feature - component, via, trace, copper pour is 40 mils (1.0 mm)”. I have a hard time with IPC spec’s and where to find out things like that. I have been using .040 for planes and .020 for traces. What spec are these things in?
I don't mean to sound stupid,
Dumb Rick |
Posted By: Tom H
Date Posted: 29 Oct 2012 at 8:55am
|
I don't get all of the rules from IPC, but they do document a lot of DFM stuff in the IPC-2221 and IPC-2222. I use fabrication shops and common sense most of the time. Example: I went to Google and typed "DFM Guidelines" and I found this PDF file - http://irtfweb.ifa.hawaii.edu/~ao/Electronic/Peter_dump/Electronics/System/Text/PCBCADGuidelines.pdf" rel="nofollow - http://irtfweb.ifa.hawaii.edu/~ao/Electronic/Peter_dump/Electronics/System/Text/PCBCADGuidelines.pdf This document produced in Hawaii surveyed several California Fabrication shops -
There are comparisons between manufacturers. You say to pull your planes back 40 mils but traces 20 mils. To me this means that you have traces without a reference plane below them. I wouldn't do that. The main reasons why features need to be pulled back from the board edge is the answer to your question. Is it because the fabrication shop is V-scoring or using a router. When breaking up the panel into individual boards, V-Scoreing can leave rough edges that need to be panelerized plus the process requires recessed features as not to damage them. Does your panel need to remain intact for assembly? If so, there will be breakaway rat-bite holes in the router process. |
Posted By: rdl86626
Date Posted: 29 Oct 2012 at 9:07am
|
Thanks Tom,
Thank you very much and I see your point. We have boards that are ridgid flex with analog /digial mixed. I have 1 or 2 traces that break that rule, which I do break if I have to, like you say common sense is the best rule. Thanks again. not so dumb Rick |