PCB Libraries Forum : Odd Looking Footprint for Chip Array https://www.PCBLibraries.com/forum/ Mon, 06 Apr 2026 17:44:01 +0000 Wed, 29 Aug 2012 08:23:32 +0000 http://blogs.law.harvard.edu/tech/rss Web Wiz Forums 12.07 360 https://www.PCBLibraries.com/forum/RSS_post_feed.asp?TID=510 <![CDATA[PCB Libraries Forum]]> https://www.PCBLibraries.com/forum/forum_images/PCBLForumLogo.gif https://www.PCBLibraries.com/forum/ <![CDATA[Odd Looking Footprint for Chip Array : To summarize, the significant...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1619.html#1619 Author: Tom H
Subject: 510
Posted: 29 Aug 2012 at 8:23am

To summarize, the significant differences are:

1.       Inthe Toe Goal…the manufacturer is ignoring the IPC toe

2.       Inthe Heel Goal…the manufacturer is ignoring the IPC heel

3.       LPWhas a smaller IPC toe than FPX (bug in LPW)

4.       LPWhas different place and size rounds. 0.05 mm for LPW and 0.01 mm for FPX

5.       Finally,LPW has a minimum pad-to-pad spacing rule of 0.20 mm so it’s heel is being trimmedmore than FPX which has a minimum pad to pad of 0.15 mm.

 
]]> Wed, 29 Aug 2012 08:23:32 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1619.html#1619 <![CDATA[Odd Looking Footprint for Chip Array : Sure, here&#039;s a top-level...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1606.html#1606 Author: LaserAlex
Subject: 510
Posted: 28 Aug 2012 at 1:48pm

Sure, here's a top-level link:
http://industrial.panasonic.com/www-cgi/jvcr13pz.cgi?E+PZ+3+AOC0001+EXB18V102JX+7+WW
 
The catalog with dimensions is here:
http://industrial.panasonic.com/www-data/pdf/AOC0000/AOC0000CE1.pdf
and the recommended footprint is here:
http://industrial.panasonic.com/www-data/pdf/AOC0000/AOC0000PE6.pdf
 
If you look at the image in my first post, you'll see that Footprint Expert makes pads that are half as wide and twice as long as the recommended land pattern.  The LP Wizard comes up with something pretty close to the manufacturer's recommendation.
 
]]> Tue, 28 Aug 2012 13:48:24 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1606.html#1606 <![CDATA[Odd Looking Footprint for Chip Array : Can you send us the datasheet...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1604.html#1604 Author: Jeff.M
Subject: 510
Posted: 28 Aug 2012 at 12:48pm

Can you send us the datasheet (or link) for the part you're creating so we can check it?]]> Tue, 28 Aug 2012 12:48:43 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1604.html#1604 <![CDATA[Odd Looking Footprint for Chip Array : The PCB Footprint Expert is...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1603.html#1603 Author: Tom H
Subject: 510
Posted: 28 Aug 2012 at 12:47pm

The PCB Footprint Expert is a brand new tool that was written from scratch and during the process we discovered some mistakes we made with LP Wizard.
 
Also, the new program uses a higher resolution of 0.01 mm snap grid round-off while LP Wizard uses a 0.05 mm round-off.
 
If there are differences, they should only be 1 or 2 mils.
 
]]> Tue, 28 Aug 2012 12:47:23 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1603.html#1603 <![CDATA[Odd Looking Footprint for Chip Array : Thanks, Tom.I&#039;m OK with the...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1602.html#1602 Author: LaserAlex
Subject: 510
Posted: 28 Aug 2012 at 12:41pm

Thanks, Tom.

I'm OK with the general idea of entering the manufacturer's preferred footprint.  However, it doesn't explain why PCB Footprint Expert gives a different recommended footprint than LP Wizard.  If they are both using the same version of the IPC standard for their calculations, they should both produce identical land patterns.  The fact that they don't seems like a possible bug to at least look in to.

In the mean time, I have created a footprint according to the manufacturer's instructions, I just want to make sure this doesn't cause a problem for any other users in the future.

Regards,

-Alex
]]> Tue, 28 Aug 2012 12:41:23 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1602.html#1602 <![CDATA[Odd Looking Footprint for Chip Array : With 0201 microminiature components,...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1560.html#1560 Author: Tom H
Subject: 510
Posted: 25 Aug 2012 at 8:51am

With 0201 microminiature components, less solder is sometimes best and according to the IPC-7351 mathematical model that's true.
 
However, if the component manufacturer did their due diligence and tested their recommended pattern and it passed all stress tests then I would consider using it. That is why we built into the new PCB Footprint Expert the ability to enter the component manufacturer recommended pattern dimensions.
 
Every component family has a "Footprint" tab. After you insert all the component dimensions and select "OK" to calculate the IPC pattern, select the "Footprint" tab to compare the IPC pattern with the manufacturer's pattern dimensions. If they're way off, select the "Use Manufacturer's Recommended Dimensions" button and enter the pad length, width and separation dimensions and build that pattern. The IPC rules for Courtyard spacing will be auto-calculated and the silkscreen will be auto-trimmed to follow your silkscreen to pad rule.
 
 
]]> Sat, 25 Aug 2012 08:51:33 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1560.html#1560 <![CDATA[Odd Looking Footprint for Chip Array : I was trying to create a footprint...]]> https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1559.html#1559 Author: LaserAlex
Subject: 510
Posted: 25 Aug 2012 at 2:03am

I was trying to create a footprint for a small (quad 0201) Panasonic chip array resistor.  The footprint created by PCB Footprint Expert has really skinny lands, when compared to both the manufacturer's recommended footprints and the Mentor IPC footprint calculator I got with my copy of the IPC standard.

Is this a bug, or has the standard changed?

Thanks!


]]> Sat, 25 Aug 2012 02:03:36 +0000 https://www.PCBLibraries.com/forum/odd-looking-footprint-for-chip-array_topic510_post1559.html#1559