Print Page | Close Window

Standard Chip Package Case Codes & Dimensions

Printed From: PCB Libraries Forum
Category: Libraries
Forum Name: PCB Library Construction Guidelines
Forum Description:
URL: http://www.PCBLibraries.com/forum/forum_posts.asp?TID=2440
Printed Date: 28 Jan 2023 at 10:15pm


Topic: Standard Chip Package Case Codes & Dimensions
Posted By: Tom H
Subject: Standard Chip Package Case Codes & Dimensions
Date Posted: 24 Feb 2019 at 12:33pm
Chip Resistor: 

Chip Non-polarized Capacitor:

Chip Inductor:

Chip Diode:

Chip LED:

Chip Antenna: 

Chip Polarized Capacitor:


Here is a table listing the Chip package Case Code and package dimensions for "Standard Chips"



If the Chip dimensions do not match the table then a new or different Case Code must be assigned. 

Note: there are various Heights to all of these packages, but the Height does not impact the resulting pad size for the Footprint Land Pattern. 

However, the Height is important for the 3D STEP model creation and should be included in the Footprint name. 

Also, the Terminal Lead may be a different length and that should be included in the Footprint Name because that does affect the resulting pad size. 

Here is a typical Footprint Name for a 0201 (0603 Metric) Capacitor part:

Footprint Land Pattern Name: CAPC60X32X27L15 

CAP = Capacitor
C = Chip
60 = 0.60 mm body Length
32 = 0.325 mm body Width
27 = 0.275 mm maximum Height
L15 = 0.15 mm nominal Lead Length

Notice that the Leading Zeros are ignored and only the first 2 numbers to the right of the decimal point is used in the Footprint Name. 

But the Leading zeros are in the Case Code. The Case Code = one number to the left and right of the decimal point. 

A typical Physical Description for this package will be: 
Capacitor, Chip; 0.60 mm L X 0.325 mm W X 0.275 mm H body

The EIA Inch Based Names are still widely used today in the electronics industry, even though the Metric Names created by EIAJ in Japan were first introduced in the 1980's in the PDP-100 publication. American assembly shops, EE engineers and component manufacturer's did not adapt to the metric naming convention and translated all of the original documentation from Metric to Imperial units so they could better comprehend the package sizes. This was one of the biggest mistakes in the global electronics industry and very short sited of the future of the industry. 

Today, all Standard package dimensions are printed using Metric Dimensions but the translated Inch Based package names have deep roots in the industry and have settled as the defacto standard. Now we have to deal with 2 systems of measurement rather than the supreme metric unit measuring system. 




-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn



Replies:
Posted By: Arun7290
Date Posted: 24 Mar 2021 at 10:01am
Hi,
From the above table, Is it possible to have a standardized terminal lead length for all the packages?


Posted By: Tom H
Date Posted: 24 Mar 2021 at 11:03am
The component manufacturer's will never standardize the Terminal Lead Length or the Tolerance. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: Arun7290
Date Posted: 25 Mar 2021 at 11:52am
Hi Tom,

Thanks for the reply. Can we use the above listed package sizes for Wraparound parts as well in the same case code? 

Because It is mentioned that the above case code dimensions are only for Standard Chips. 

And I am working on some wraparound packages of the standard case code. 

Can we use PCB library expert for footprint creation for these parts? 

Or Is it better to follow the Manufacturer recommended land pattern?




Posted By: Tom H
Date Posted: 25 Mar 2021 at 11:59am
Use the mfr. recommended pattern for this new upcoming component family. 

Some manufacturers use a periphery solder joint goal and other use a Toe, Heel and Side pad stack. 

This is a new Terminal Lead form that has not been fully tested by the world standards like IPC-J-STD-001 for solder joint acceptability. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: lladam
Date Posted: 02 Jul 2021 at 6:26am
Hi,

How to make a Proteus library part of MEGA2560 Pro Mini, or where can find one please.

Because the board too small to put many pins on.

Thanks


Posted By: Tom H
Date Posted: 02 Jul 2021 at 8:47am
You need to attach a link to a PDF file zipped or a URL link to the datasheet would be better. 

Then we can post the Proteus footprint. 

Are you using the Free V2021 Footprint Expert Pro for Proteus? You could create the footprint in a couple minutes. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: phil.holden
Date Posted: 07 Sep 2021 at 4:08am
As is common procedure, especially during these times with supply-chain issues. We try and specify x3 MPNs for all of our passive devices. 

As there could be 3 substituted parts fitted all with differing terminal lengths. How am i best addressing this when creating a passive library? 

This is much less of a problem for active parts and connectors that are less 'interchangeable'. 

Thanks

In addition to the above. I have noticed that the terminals sometimes overhang the pads when using 'rounded rectangle'. In your opinion, would this be a problem? 



Posted By: Tom H
Date Posted: 07 Sep 2021 at 9:08am
To get 3 or more passive packages to fit into the same Footprint, find parts with the same dimensions and tolerances. If the package dimensions are the same but the tolerances are different, then round the tolerances off so that they are all the same. 

Rounded Rectangle Pad Shape: You should change your Maximum Radius from 0.25 to 0.15 or 0.10 or something smaller. 

Change this setting in "Tools > Options > Pad Stack Rules > SMD Corner Rounding > Corner Radius Limit". 


-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: phil.holden
Date Posted: 08 Sep 2021 at 5:26am
Hi Tom,

For my Enterprise Edition CLOUD Licensed the options under Pad Stack Rules are 'greyed' out. Does this mean that i am unable to control this globally? 


Posted By: Tom H
Date Posted: 08 Sep 2021 at 8:32am
Read the User Guide in the main installation folder under "Documents". 

  • Charter 1 Footprint Expert Console Options
  • Charter 2 Footprint Expert Calculator Options - Pad Stack Rules
  • Charter 3 Footprint Expert Calculator Options – Drafting
  • Charter 4 Footprint Expert Calculator Options – Fiducials
  • Charter 5 Footprint Expert Toolbar Icons and Menu Options
You cannot edit the program Master Options. You need to create your personal option files (as many as you want). 

Select File > Save As > Your Master Options .opt



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: AnonAnon
Date Posted: 07 Feb 2022 at 5:41am
Hi Tom,

Please excuse me if you've answered this a thousand times but I'm looking to find which standard defined the "Least" and "Most" limits for each footprint. I can see IPC-SM-782 defines the nominal and references equations in a section 3.3? I am happy to purchase the standard but wanted to ensure it contained the correct information before I purchase.

Do the IPC standards only provide the nominal and one has to calculate the limits?

Kind regards,

David


Posted By: Tom H
Date Posted: 07 Feb 2022 at 10:01am
IPC-7351B contains the 3-Tier Density Levels for Land Patterns. 

However, that document is 12 years old and out of date and it took information from the 1987 IPC-SM-782 which is obsolete.

The solder Joint values are way too robust for today's technology. 

Footprint Expert solder joint goals are derived from IPC J-STD-001 standard as it's the main standard that all other standards are built upon. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn



Print Page | Close Window