| FreePCB User Guide | Version 1.2

PREV | Table of Contents | NEXT

6. Footprints and Libraries (continued)

6.2 Footprint Wizard

There will be times when you need a footprint that is not in one of the libraries that come with FreePCB. The Footprint Wizard is a tool for generating footprints for a variety of standard packages. It is invoked with the Tools > Footprint Wizard menu item. This pops up the following dialog:

A footprint is created by setting the various controls in the dialog. These are described below:

- Name - This is the name which will be assigned to the footprint when it is saved (e.g. DIP28 )
- Type - The type of package. A line diagram of the selected type will be shown in the dialog (QUAD in the example above)
  - SIP (for Single Inline Package) - this consists of a single row of one or more pins
  - DIP (for Dual Inline Package) - two rows of pins, numbered as for a DIP IC package
  - QUAD - four rows of pins arranged as a rectangle (as shown above) and numbered as for a PLCC or QFP package
  - HEADER - pins arranged in a grid and numbered sequentially by column
  - HEADER2 - same as HEADER except pins numbered sequentially by row
  - PGA/BGA (for Pin Grid Array or Ball Grid Array) - pins are arranged in a rectangle, and named using the convention for grid arrays
- Units - mils or mm
- Number of pins
  - Total - the total number of pins in the package
  - Per horizontal row (for QUAD, HEADER and PGA/BGA packages only) - the number of pins per horizontal row
  - Per vertical row (for QUAD, HEADER and PGA/BGA packages only) - this is filled-in automatically, for information
  - Pin 1 position (for QUAD packages only) - there are three options:
    - top row, center pin
    - bottom row, left-most pin
    - top row, left-most pin
- Pads
  - Shape - there are four options:
    - Rectangular - rectangular pads
    - Pin 1 square, others round - a square pad for pin 1, others round
    - Round - round pads
    - Square - square pads
    - None - used to create a hole without a pad (for a mounting hole, for example)
  - Hole diameter - the diameter of the hole in the pad for through-hole pads (blank or "0" for SMT pads)
  - Width (X) - the pad width (shown as "X" in the line diagram)
  - Length (Y) - the pad length (shown as "Y" in the line diagram)
  - Spacing (E) - the center-to-center spacing of pads within a row ("E" in the line diagram)
- Distance between top and bottom rows - by selecting one of the three radio buttons, this distance can be set as:
  - Inner-inner (G1) - the distance between the inner margins of the pads ("G1" in the diagram)
  - Center-center (C1) - the distance between the centers of the pads ("C1" in the diagram)
  - Outer-outer (Z1) - the distance between the outer margins of the pads ("Z1" in the diagram)
- Distance between left and right rows - by selecting one of the three radio buttons, this distance can be set as:
  - Inner-inner (G2) - the distance between the inner margins of the pads ("G2" in the diagram)
  - Center-center (C2) - the distance between the centers of the pads ("C2" in the diagram)
  - Outer-outer (Z2) - the distance between the outer margins of the pads ("Z2" in the diagram)
- Preview - clicking this button creates a preview of the footprint in the dialog

The best source for the dimensions of a particular package is the manufacturer's datasheet. This is usually available on the Internet. In some cases, the manufacturer will even supply a drawing of the suggested PCB footprint (for SMT parts, these are often referred to as "land patterns").

After you have entered the settings for the footprint, click on Preview to see an image of the footprint. If it looks OK, you can save it to a library file by clicking Save. This will pop up the Save Footprint dialog, shown below.

The Footprint name is copied from the Wizard, and can be changed here if you like. The Author, Source and Description fields may be filled with text describing the footprint. The Library file list box allows you to select a library file, or enter a new file name to create a new one. It will be initialized to user_created.fpl.

Several examples of footprints created with the Footprint Wizard are given below.

6.21 Example 1: Mounting Hole or Test Point with a single pin

To create a single-pin footprint for a mounting hole or test point, set the Type to "SIP" and the Number of pins to "1". The settings for a mounting hole with a hole diameter of 100 mils and a round pad with a diameter of 200 mils are shown below.

6.22 Example 2: Resistor with Axial leads

Let's start with a drawing of the resistor, taken from the Panasonic datasheet. This footprint will be for the 1/4 watt type ERD25.

From the datasheet, the package length is 6.35 mm. To allow for bending the leads, we will space our pads 12.5 mm. apart. The lead diameter is 0.60 mm. To allow clearance for insertion, the hole diameter will be 0.9 mm. The pad diameter will be 1.4 mm. The Footprint Wizard settings are shown below.

6.23 Example 3: DIP package with rectangular pads

Here are the settings for a DIP IC footprint with 20 through-hole pins. The standard DIP package pin spacing is 100 mils and the row spacing is 300 mils. We will use rectangular pads 80 X 40 mils in size with a 25 mil hole diameter.

6.24 Example 4: QFP package with 100 pins

This footprint is based on the package for the Cypress CY7C1329, a 64K X 32 synchronous cache RAM. The package dimensions are shown in the drawing below, which was copied from the Cypress datasheet.

For the footprint, we want the pads to extend 0.5 mm beyond the end of each pin, so we will add 1.0 mm to the external dimensions of the pin rows. Also, we have turned the package on its side so that pin 1 is in the lower-left corner. The settings for the Footprint Wizard are shown below.

PREV | Table of Contents | NEXT