BoardSurfers: Training Insights: Creating Footprints in Allegro PCB Editor

A footprint is a graphical representation composed of pads used for connecting electronic devices to a PCB. Any error while creating a footprint can cause redesigning of the whole board. Therefore, creating the right footprint is important to the design and manufacture of reliable PCBs. You can create footprints in many ways using Allegro® PCB Design applications.

For creating standard-compliant footprint symbols, Allegro PCB Editor offers Symbol Editor, an integrated library-development environment. The user interface of Symbol Editor makes part creation fast and easy by providing specific symbol-creation commands, powerful wizards, and templates. You can create a new symbol from the scratch or modify existing symbols.

In this blog post, we will go through all the necessary steps to manually create a dual in-line package (DIP) symbol using the symbol editor mode of Allegro PCB Editor.

How to Create Footprint in Allegro Symbol Editor

To create a new footprint manually, do the following six generic steps:

Create a new drawing

1. To start Symbol Editor, launch Allegro PCB Editor and choose File ─ New.
2. In the New Drawing dialog, select Package symbol as Drawing Type. Browse to the symbol directory location and name the drawing, say as dip16.

You are now in symbol editor mode and see a blank canvas where you can create the new symbol.

Before creating symbols, you should specify drawing extents and design parameters.

3. Right-click anywhere in the design canvas and choose Quick utilities ─ Design Parameters. Select the Design tab and set parameters in the Design Parameter Editor.

 Add and configure pins

1. Ensure the PADPATH variable is set to the correct directory path in your env file.

To assign pins, Symbol Editor searches the padstack directories defined by the PADPATH environment variable.

2. Now to add pins, choose Layout ─ Pins.

The Options tab has various fields. Set up the fields to create the desired package.

• For electrical pins, choose Connect. If you choose Mechanical, you cannot assign a net to it because it does not have a pin number.
• In the Padstack field, enter the padstack name by typing it or using the padstack browser. You can choose the same or different padstacks for all the pins.
• Set Copy Mode to Rectangular. The other option is Polar which creates pins in a circular pattern.
• X specifies the pin columns and Y pin rows. You can add multiple pins that use the same padstack.
• Specify pin to pin spacing. The Order determines the direction of pin placement as upwards or downwards.
• Do not change Pin #. It determines which pin number to start the numbering from.
• Offset values are used to specify how far is the pin number located from the pin.

3. Click anywhere in the design canvas to place the pins.
4. Place the next set of pins either by clicking on the canvas or by specifying the coordinates in the Command window.
5. If you want to change any pin, say from circular to square, you need to change the padstack. Choose Tools ─ Padstack ─ Replace. In the Options tab, select the old padstack you want to replace or type the pad name. For assigning a new padstack, either type the pad name or browse for the new replacement. In the Pin#(s) field enter the pin number you want to change and click Replace.

 Add component outlines (Silkscreen and Assembly)

The silkscreen layer contains the labels and outlines of the component. To add silkscreen as line or arc elements, do the following:

1. Choose Add ─ Line or Add ─ Arc w/Radius.
2. In the Options tab, select Package Geometry class and Silkscreen_Top subclass.
3. Enter a Line width value and draw a silkscreen.

 In case you cannot see grids, go to Setup ─ Grids. In the Define Grid dialog box, check the Grids-on checkbox.

You can create assembly outline in the same fashion. It contains information about the placement and orientation of all the components in the board design. To add assembly outline, do the following:

1. Choose Add ─ Line or Add ─ Arc w/Radius.
2. In the Options tab, select Package Geometry class and Assembly_top subclass and draw the assembly outline.

Define constraint areas (package boundary and package height)

To define areas, do the following:

1. Choose Setup ─ Areas.
2. Create a package boundary that checks for package overlap and is used during placement.
   • In the Options tab, select Package Geometry class and Place_bound_top
   • Draw a polygon as a package boundary.
3. After adding package boundary, choose Setup ─ Areas ─ Package Height to add package height restriction.
4. Select the package boundary area and specify either maximum or minimum height in the Options tab.

Add labels

Labels are placeholders for displaying component data such as assembly and silkscreen reference designators and device types. You must define at least one reference designator to successfully create a footprint.

Choose Layout ─ Labels ─ RefDes and use the Options tab to specify the location and text block size. The text block controls the size of the label. You can add reference designators to the silkscreen and assembly layer separately.

Save symbol files

Your footprint is ready to save. Check the status in the Command window. It says two files are created, dip16.dra and dip16.psm. The .dra file is a graphic file used for editing purposes only. The .psm  file is the binary equivalent of the drawing file, created by default when you save the symbol. This file contains a compiled version of the symbol which has layer details and is used by placement utilities.

 Allegro PCB Editor makes it easy to create a new symbol that you need to use in your design. I hope this blog helps you quickly get started to successfully create a footprint!

To learn in detail about this flow, watch the How to create a Footprint using the Allegro® PCB Editor training byte on the Cadence Support portal. Click the training byte link now or visit Cadence Support and search for this training byte under Video Library.

Cadence Training Services now offers a Digital Badge for the popular training courses. These badges indicate proficiency in a certain technology or skill and give you a way to validate your expertise to managers and potential employers. You can add the digital badge to your email signature or any social media platform, such as Facebook or LinkedIn, to highlight your expertise.

To know more, see the blog post Take a Cadence Masterclass and Get a Badge.

You might also be interested in the training Learning Map that guides you through recommended course flows as well as tool experience and knowledge-level training modules. Do SUBSCRIBE to be updated about upcoming training modules. If you have any questions about courses, schedules, online, public, or onsite live training, then reach out to Cadence Training.