Documentation

PCB Footprint Editor

7 min read

Using the footprint Editor, create or edit a footprint that will be referenced from the Part and called for use in a PCB design.

Alternatives to manually creating a Footprint

As well as manually creating a footprint using the built-in footprint editor, you can also use the Footprint Wizard, or import footprints from other external resources, such as PCB Libraries.

Creating a new basic footprint

Footprints can be quite complex and contain different facets. The description below will concentrate on a basic footprint to start with, and additional sections below adding special features and details to it.

Getting Started

From the New dialog, a PCB footprint editor session will begin. You can also specify the PCB Technology file to be used.

This will form the basis of a new PCB footprint. If [None] was used for the Technology file, you can create your own styles and rules using the Technology dialog. These can be saved for later use with the PCB design if required. Using [None] is not recommended as it means you start with no real structure to the technology; better to start with one of the supplied examples and save it as you create your own styles.

Adding Pads

Within the Footprint, you can add different types of Pad. Each type of pad type is used for a different purpose:

  • Component Pads
    Pad - Use this option to add through-hole component pads to your footprint.
    SMD Pad - Use this option to add surface mounted component pads to your footprint.
    Both of these pad types are numbered and are included in the overall pad count for a Part.

  • Mounting Holes - these are a specific pad type and have no pad numbers so they do not included in the overall pad count for a Part.

  • Free Pads - these are floating (non-component) pads. Use them for any special situation where Component Pads, Mounting Holes or Vias are not appropriate. They are available but less used in a footprint.

  • Pads used for Chip On Board design (requires license)
    Die Pads - A Die Pad is added to define the location of the bare die in the design. This is a fixed pad a bit like a normal footprint and cannot be moved once used in the design. Once added, a ‘paired’ Bond Pad will be added along with a connecting Bond wire.

    Bond Pads - When a Die pad is added, a Band Pad will also be added automatically as part of the pairing.

Adding footprint detail

Once the footprint editing session has started, you should now add pads. From the Insert > menu, select Pad or SMD Pad.

Pad Styles

The default pad style will be used but you can select another style using Change Pad Style option from the shortcut menu.

Pad Number Sequencing

Before saving a Footprint, ensure that all component pads added are numbered sequential without any gaps in the sequence. Failing to do this will result in an error message when you try saving the footprint to your library.

Placing pads

With the pad on the end of your cursor you can position it where required. Use a Grid or Construction line to guide you. Alternatively, position the pad using the coordinates displayed on the status bar, relative coordinates and delta coordinates.

Placing and rearranging multiple pads

Multiple pads can be placed at the same time to create your footprint pattern. You can do it by adding one pad and copying and placing it multiple times using the replicate option, or adding multiple pads and repositioning them into the pattern required using the Rearrange Multiple Pads option.

Using grids to position pads

Visible Grids enable you to snap pads onto standardised positions, such as a 0.5mm grid or a 100thou/Mils grid. different grids can be set up and changed using Change Grids.

Using construction lines to position pads

As well as grids, you can also use Construction Lines to position pads. Construction lines are still used when manually moving pads, but it means pads can be snapped to visible lines and intersection points.

Adding a Symbol Origin

In most cases, there are two main ‘Origins’ -

  • A Symbol origin which defines the origin when the component is placed in the design. This is the point used when you place or moved the component. When adding the first pad or shape, this origin is automatically added. It can be moved manually to you required position. By default, Pulsonix uses the symbol origin on Pin 1 if through-hole technology, and the centre of the footprint if a surface mounted component.
  • The component Name origin. This is when the Component name is located in the design. It also defines the layer that it appears on.

Adding a Component Name Origin

Use Insert Component Name to add the origin that will be the location used in the design to display a component name, such as R1, U1, IC22 etc. This will also have a Layer defined and is usually on the Silkscreen layer.

Adding Shapes & Areas

Shape items can be added for uses such as documentation and Silkscreen identification, and Areas used during component placement, for use in 3D, or keepout of various items.

Use Insert Shape option to add documentation shapes such as Silkscreen or Assembly detail. When adding these, you will need to choose the layer that they belong to.

Use Insert Area to add Areas that will be used for Component Placement, Board Cutouts, Keepout Areas, Copper Pour Keepout etc. When adding these, you will need to choose the layer that they belong to. Once added, use Area Properties to change details on its use.

As well as shapes and areas, you can also use the Insert Copper option to add free copper areas to your footprint.

Adding Attributes & Attribute Positions

As well as the Component Name origin (which is an unsatisfied attribute at this point [an attribute position with no value]), you can also add attribute positions using the Insert Attribute Position option.

Adding Text

You can add text to your footprint using the Insert Text option. This is not the same as the Component Name; this is free text to add documentation detail. When adding text, you will need to choose the layer it belongs to.

Saving the Footprint to your library

Once your footprint has been created as required, and the component pads are all sequentially numbered, use the Save To Library option from the File menu to save it into your library. From this dialog, you can define its name and which library it will be saved into.

Advanced Footprint Details

Additional features can be added to footprints:

Adding Breakouts

Breakouts can be used to define fanout patterns. Use the Insert Breakout option to add breakouts. These then get converted to tracks when the component is used in the design. When adding breakouts, a Via is automatically added to its end.

Adding Vias

Free vias can be added to the footprint using the Insert Via option. For example, if you wish to create a via in pad (VIP) to predefine your via location. If doing this, you must also change the association between the via and its host pad. Use the Add To Net option from the context menu to do this. Make the net name the same value as the pad number (or ensure net names on the pad and via match). An additional property to change is on the Component Via Properties page; select the No Spacing Errors Within Footprint check box to prevent the Component Via from producing design rule errors against other items within the same Footprint.

Adding Wires

Wires can be added if creating a jumper component. Use the Insert Wire option.

Adding Die and Bond Pads

If you have the Chip On board option, you can add Die and Bond pads to the footprint.

When using the Insert Die Pad option, a wire and paired Bond Pad are also automatically added. When adding Die and Bond Pads, you will need to choose the layer they belongs to.

PCB Technology | Layers | Pad Styles | Line Styles | Track Styles

Backlinks