Jumpers, also referred to as wire links, allow you to replace routing with a Jumper component, which is often an essential ingredient to successfully designing a single-sided board.
Early printed circuit boards were all single sided. To successfully implement all of the connections, jumpers or wire links were often used to create another layer of connectivity, which could pass across the printed routing. The image below shows an example of Jumpers being used to implement the routing on one side of the board.
Note the representation of a Jumper, with a curved connection line between the two pads. In the image, the jumper connection lines are shown in different colors because they inherit the color assigned to the net.
To act as a jumper, you need:
After placing a Jumper in the workspace you will need to set the Net attribute of one of the pads manually in the Properties panel since there is no automatic net inheritance. Note that if the component is defined as a Jumper, then the other pad will automatically inherit the same Net name.
The View menu includes a Jumpers sub-menu that allows control over the display of Jumper components.
There are also Jumper sub-menus in the Netlist popup menu (N shortcut).
The query keyword
IsJumperComponent is available for filtering and rule definition.
Jumpers are typically pieces of tinned copper wire that are bent to the correct length, meaning they need to be in the BOM. To support this, Jumpers also can be included on the schematic so that they are included in the Bill of Materials. The Synchronizer and the Report engine have the following behavior for synchronizing Jumpers:
The following description is one approach to working with Jumper components. This workflow starts at the schematic, but you can also start by placing the Jumper footprints directly onto the PCB. The main reason for starting on the schematic is that when the design is transferred to the PCB workspace, the footprints will have the correct component Type of Jumper. If you place them directly from the PCB library into the PCB workspace, the component Type will default to
Standard, so you will need to manually set it.
Create a footprint for each length jumper that will be used. Typically jumpers are designed in pre-defined lengths, for example, in increments of 0.1 inch (100 mils).
As mentioned above, there are two conditions that make a Jumper a Jumper:
Jumperin the Properties panel. Note that this can only be set once the footprint has been placed into the PCB workspace; it cannot be set in the PCB Library editor.
The image below shows a typical Jumper in the PCB Library editor. Both pads have the Jumper value of
On the schematic side, you can either:
Once the symbol has been created:
Once the Jumper has been designed, you can place a number of them onto the schematic. At this stage, you probably do not know how many you will need, however, extras can easily be deleted. Keep in mind they are on the schematic to ensure they go into the BOM; they do not need to be wired into the circuit at each location that they end up being used. For that reason, it makes sense to place them all on the same schematic sheet, perhaps with other BOM-only hardware, such as screws.
When a Design » Update PCB Document command is performed, all of the jumpers will be placed into the PCB workspace using the default footprint to the right of the board shape.
The image below shows the PCB, almost completely routed. Note the remaining connection lines showing where the routes are not complete. There are also a number of un-placed Jumper components to the right of the board.
The routing for each of these connections cannot be completed because there is no route path available on this single-sided design. To complete them, the Jumper components will be used.
To complete a connection with a Jumper: