Chip Resistor: 

Chip Non-polarized Capacitor:

Chip Inductor:

Chip Diode:

Chip LED:

Chip Antenna: 

Chip Polarized Capacitor:

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. 

From the above table, Is it possible to have a standardized terminal lead length for all the packages?

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. 

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. 

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? 

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. 

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

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? 

• 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

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

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.