I've come across the the symbols for closed solder jumpers in design libraries, and now I came across one in a design. I get why you might include an open jumper that could be solder closed, but what is the use case for a solder jumper that is already closed in the pcb layer?

An example of the symbol: Solder jumper closed symbol

  • \$\begingroup\$ Is it closed in the actual footprint, or just in the schematic? \$\endgroup\$ Commented Dec 23, 2018 at 17:45
  • 2
    \$\begingroup\$ above it appears to be used for write protect, closed during manufacture so the rom can be written then opened to protect the contents, but closable using solder if the rom needs to be rewritten. \$\endgroup\$ Commented Dec 23, 2018 at 19:34
  • \$\begingroup\$ In a sense, you answered your own question. "I get why you might include an open jumper." If you get that, then you also get why you might want to close it. You might be thinking that jumpers should always be user-servicable. Sometimes those jumpers distinguish between models of the same device with differing capabilities - capabilities that are permanently activated or deactivated with a solder jumper and are never meant to be fadiddled with. \$\endgroup\$
    – JBH
    Commented Dec 23, 2018 at 21:52

3 Answers 3


In this case write protect is optional. And disabled by default.
Cut the trace if you want to enable it, link by solder to disable it.

Sometimes you have a need for normally closed solder jumpers.

Sparkfun: How to Work with Jumper Pads and PCB Traces

  • \$\begingroup\$ In this context it is also common to see both PU/PD on a logic line and one not populated. In this case the designer chose to have a PU and Jumper. One reason this is done is that changing the default only requires removing a part instead of removing and replacing a part (and possibly having the wrong value accidentally). \$\endgroup\$
    – crasic
    Commented Dec 23, 2018 at 18:40

In addition to the specific explanation that @Jeroen3 provided for your example, there is at least one additional purpose of this type of jumper (Note that the symbol can also be reused for more general jumper purposes and not only the solder-jumper footprint)

Serve as a "net-tie" (Term from altium).

If you have say, AGND and DGND , or GND and SHIELD and want to make certain that they are connected together at exactly one point (and not common net which prevents you from using DRC to review the ground separation), you may use a closed solder jumper to do this if the EDA does not have a special element.


Jeroen3 is absolutely correct. As for a common use case, think about it as the option for a (semi-)permanent switch. It's somewhat similar to placing 0R resistors in places you might want to break the connection later.

A company I worked for had developed at least one board where there were 2 of such NC solder jumpers. Both led to input pins on the uC. That board was roughly 9 out of 10 times used for a specific function and the remaining times as a gateway to such boards. Those gateways had a little extra hardware on them, but that extra hardware needed to be tested manually after production.

One of those NC solder jumpers would be cut at the end of the test procedure to indicate both that this was a special board and that the special features were operating successfully. The uC would no longer receive a high-input on the cut line and now everybody including the uC would know the product is safe to be used.

The other line was used in case a board had been modified in such a way it was no longer fit for use in the field. Think of demo-applications and testing rigs. Those boards were no longer fit for sale.

There are probably many, many more (ab-)uses possible.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.