1. Design

    a. Units

• There are 4 options for units, but millimeter is the most popular today because most package dimensions in manufacturer datasheets are displayed in millimeter units.

    b. Decimal Place Accuracy > Minimum / Maximum

• Most PCB library parts are created in millimeter units to match the current package datasheet, but everyone is in a different environment. The new "Units" allows you can set the Minimum and Maximum rounding values.

By setting the Minimum and Maximum values, you establish the program rounding values.

Example 1: using 2 place Minimum accuracy, entering a 0.8 value, will display as 0.80. The Footprint Expert will automatically add a trailing zero to round the value 2 place minimal accuracy.

Example 2: using 2 place Maximum accuracy, all values will be rounded up to the nearest 0.01. Entering a 0.025 value would display as 0.03.

The program default settings are Minimum 2 and Maximum 3. Because the minimum is 2, and will automatically remove all training zeros past 2 places. The maximum setting of 3 will only round up values less than one micrometer.

Example 3: using a 3 place Maximum accuracy, a value of 0.3255 will be rounded up to 0.326

Example 4: using a 2 place Minimum accuracy, a value of 0.29 will be rounded up to 0.30

The most important thing is that both the minimum and maximum options go up to 6 places. This accuracy is intended to increase the rounding accuracy when converting between Metric and Imperial units. It is not recommended to select 6/6 as the min/max, because this will affect the Physical Description that is auto generated by Footprint Expert in the FPX file. Having every value 6 places to the right of the decimal point would also affect every component family calculator, as every value would be rounded and displayed with 6-point accuracy. A simple value of 0.01 would display as 0.010000 and the Physical Description would be the same.

The same concept works the same for all 4 Unit Options.

    a. Calculated Footprint > Pad Size and Pad Place

• 3 = 0.001
• 2 = 0.01
• 1 = 0.10

2. Design Options also include these settings:

    a. Footprint Naming Convention
        This feature has 3 options:

• PCB Libraries (originally intended for IPC-7351C)
• IPC-7351B
• IPC-7352

The PCB Libraries option is an updated Naming Convention that was submitted by PCB Libraries, Inc. to IPC 4 years ago and intended for the IPC-7351C release. The IPC-7351C land pattern sub-committee voted to approve it, but in 2023, the committee leaders decided to revert to the legacy IPC-7351B naming convention.

The main differences between the 3 naming conventions are that IPC-7351B produced mass duplication of land pattern names because it did not contain Thermal Tab sizes, Terminal Lead sizes, BGA ball sizes, and it was not 100% symmetrical. PCB Libraries naming convention eliminated duplication of land pattern names.

    b. Create Footprint Name Using (Units)
This feature auto-generates the name using the package dimensions inserted into the calculator. The footprint name normally uses all Nominal Dimensions except Height is always Maximum. The dimensions include these parameters:

• Component Family Abbreviation
• Pin Quantity only if there are more than 2 pins (exception for DFN as they only have 2, 3 or 4 pins)
• Pin Pitch only if there are more than 2 pins
• Lead Span for parts with leads that protrude outward
• Body Length and Width for Chips and Bottom Terminal Components (BTC) packages
• Height Max
• Lead Length X Width
• Thermal Tab Length X Width

IPC-7351 Guideline recommends all footprint names in millimeter units and all values are 2 places to the left and right of the decimal point. Example: A value of 7.6 will appear in the pad stack and footprint name as 760. Leading zeros are never added, and trailing zeros are always added.

    c. Density Level (suffix)

This feature has 2 purposes. It defines the global Density Level for all footprints, and it defines the footprint name suffix L, N or M to identify the density level.

• Least density level produces a smaller land pattern which includes the pad size and the courtyard. It could also impact the solder screen legend line width if you set that up in Calculator Options. The Least density level is most widely used for hand-held devices, very densely populated PCB placements and RF applications where minimum copper is required for optimal performance.
• Nominal density level produces an average land pattern suitable for Class 3 fabrication and assembly.
• Most density level produces the maximum pad size. The best probable use for the Most density level is manual soldering. However, some seem to think that Most density has an application for space systems, military weapons or critical medical devices. There is no conclusive proof or evidence that the Most density is better than the Nominal density as far as stress, vibration, and thermal cycle testing.

Note 1: The original IPC-7351 solder joint goals created in 2004 and published in 2005 were too robust for introducing a new 3-Tier library system. An example of this was the solder joint goals for Chip packages. IPC-7351 has a Nominal Density level Toe value of 0.35 mm for all chip packages. The 01005 chip resistor has a body size of 0.40 L x 0.20 W x 0.13 H. The IPC-J-STD-001 indicates that the chip toe fillet for Class 1 & 2 should be "Wetting is Evident" and for Class 3 should be 25% of the package height or 0.50 mm, whichever is Less. But the 01005 chip is not a good example because it was introduced 7 years after 7351 was released. The popular 0402 capacitor is 1.00 L x 0.50 W x 0.80 H and the resistor height is 50% less at 0.40 H and was introduced in 2000. The Toe solder joint fillet only needs to be 0.20 to meet IPC-J-STD-001 solder joint acceptability. A 0.20 Toe solder joint goal is good for both the Capacitor and Resistor 0402 package.

Note 2: The IPC-7351 solder joint goals for Least Nominal & Most are too robust between the density levels. This creates a situation where the Most density had too much solder and the Least density did not have enough solder. PCB Libraries, Inc., in conjunction with our customers determined that a more subtle variation worked much better. Example: for almost every terminal lead form for the Toe solder joint calculation, IPC-7351 starts at Nominal and adds 0.20 to the Most and reduces Nominal by 0.20 for the Least. We concluded that a variation of 0.10 between Nominal and Most and Nominal and Least is better. Too much solder generated by oversized pad stacks causes soldering problems and damage to the final assembly. Not enough solder causes performance problems and may not pass stress, vibration and thermal cycle testing.

Note 3: Regardless of all our research and the IPC-J-STD-001 Standard, we can only generalize the most common values for solder joint goals in the Footprint Expert. You have access to every solder joint goal to edit every value and create highly customized pad stacks for your electronics application.

    d. Replace Density Level Suffix With...

• This feature is primarily used for adding characters to the end of a footprint name when creating library parts with a specific Options file for a specific procedure or a specific manufacturing process. Example: FLEX (FX), WAVE (WAV), RF

    e. Pad Stack Naming Convention

• See IPC-7352 for the pad stack naming convention.

    f. Create Pad Stack Name Using (Units)

• This feature auto-generates an IPC-7352 approved pad stack name. IPC-7352 also recommends that the pad stack names be created in millimeter units with the same format.

    g. Ignore Manufacturer's Footprint Dimensions (for Batch Builds)

• This feature is primarily used for ignoring any manufacturer recommended dimensions in the FPX file when using the Batch Build feature.

    h. Include Suffix in Footprint Name

• This is turned on by default specifically to add the Density Level character L, N or M (for Least, Nominal or Most), but if you are always using one density level for your entire library, you may want to drop the suffix from the footprint name.

    i. Generate Solder Mask

• This is turned on by default. But some CAD tools auto-generate their own solder mask in Preferences and therefore there is no need to add solder mask in the pad stack with the Footprint Expert.

    j. Generate Surface Mount Paste Mask

• This is turned on by default. If you want to create a CAD library without paste mask, uncheck the box.

    k. Generate Through-hole Paste Mask

• This is turned off by default. Use this feature for PTH Pin in Paste solder process.