Home > Community > Blogs > PCB Design > customer support recommended implementing jumpers in allegro pcb editor
Login with a Cadence account.
Not a member yet?
Create a permanent login account to make interactions with Cadence more conveniennt.

Register | Membership benefits
Get email delivery of the PCB Design blog (individual posts).


* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

Customer Support Recommended - Implementing Jumpers in Allegro PCB Editor

Comments(0)Filed under: PCB Layout and routing, PCB design, PCB Editor, vias, jumpers

Over the time, jumpers have found their importance in multiple applications. The following blog is aimed to provide more insight on their usage and implementation using Cadence Allegro PCB Editor.

What is a jumper? A wire jumper is typically a short wire used to electrically connect two points. On occasion, a wire jumper is necessary on a single-sided PCB to continue the signal connection over a group of etch traces. The wire jumpers are available on tape and reel, and can be cut and formed to custom sizes with a resistor forming machine.

Creating a Jumper Package Symbol

A jumper is created as a package symbol with the jumper option enabled in the Design Parameter. The jumper symbol must only contain two via padstacks and a refdes label. Optionally, the jumper may contain place bound, silkscreen, and assembly graphical outlines or text.

Note: If a place bound shape is not defined in the jumper symbol, the application will use the jumper symbol drawing extents when the jumper is placed in the design.


You should adhere to your company's standards for naming conventions as well as any specific manufacturing criteria. For each jumper, you should have the following physical data:

  • Lead-to-lead spacing
  • Drill size
  • Pad size

Defining the Drawing Type

All commands listed here are described in the Allegro PCB Editor and Package Physical Layout Command Reference.

1. Choose File - New and choose Package Symbol

2. Enter a file name in the Drawing Name field

3. Choose Package symbol from the Drawing Type list box, and choose OK

4. Select Setup - Design Parameters

5. Select the Design tab on the Design Parameter form

6. Select Jumper in the Drawing type field of the Design Parameter form, and choose OK


Defining the Via List

1. Select Setup - Constraints - Physical

2. In the Physical Constraint Set workbook, click All Layers

3. Scroll to the right until the column labeled "Vias" is visible

4. Click in the Vias cell

This invokes the form "Edit Via List" as shown below:

5. Double click on a via in the ‘Select a via from the library or the database' field

The via populates the Via List field.

6. If more than one via is listed in the Via List field, then select the newly added via and click the Up button to move the via to the top of the Via List field. Optional elements in the jumper symbol:

While the only mandatory elements in the jumper symbol are two vias and a placeholder for the reference designator you can add additional elements to the symbol, just as you do with regular package symbols, that meet your companies design standards. These elements could be:

  • Place bound shape 
  • Silkscreen outline
  • Assembly outline

Adding a jumper symbol while routing:

The following steps can be implemented to add/place a JUMPER symbol while routing the board file.

1. Select Route > Connect (add connect command)

2. In the Design window, click on the element (pin, via, or etch segment) from which you want to start adding etch

3. Choose the right mouse button Add Jumper selection to add the jumper while routing. Ones that are grayed out either do not exist as a symbol or are not in the PSMPATH

This will place the jumper down at the current location and allow you to dynamically rotate the second via around the first. Once you perform a second pick, the jumper will be instantiated in the design.

Refer to the app note here for the detailed step-by-step procedures on the dimensioning functionality, as well as various other aspects that are not covered in this blog.

Note: The above link can only be accessed by Cadence customers who have valid login credentials for Cadence Online Support (http://support.cadence.com).

Naveen Konchada
Cadence Customer Support


Leave a Comment

E-mail (will not be published)
 I have read and agree to the Terms of use and Community Guidelines.
Community Guidelines
The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.