1
\$\begingroup\$

I have a question about power supply design for a board which use an LPC1768. Below image is taken from http://www.nxp.com/documents/other/IAR_LPC1768_Eval_Board_Schematic.pdf document.

There is a symbol in this schematic named "CLOSE". I want to be clear about what it is. My guess; it's the bridge connection between power planes for analog and digital. But I want to be sure before I start to do my design.

Please help, thank you.

IAR LPC1768 Evaluation Board Power Supply

\$\endgroup\$
3
  • \$\begingroup\$ That's like touch sensor symbol but I think it is a switch (such as jumper). \$\endgroup\$
    – Roh
    Jul 24, 2014 at 18:23
  • \$\begingroup\$ Touch sensor in a power supply? And it doesn't seem like a switch to me since it uses two separate "CLOSE" for analog ground and power. \$\endgroup\$ Jul 24, 2014 at 18:25
  • \$\begingroup\$ I didn't say that certainly that's a touch sensor. I said that's look like the symbol of it. probably that's jumper. \$\endgroup\$
    – Roh
    Jul 24, 2014 at 18:29

3 Answers 3

4
\$\begingroup\$

Yes, those are solder jumpers. They basically allow you to jump the two connections using a solder blob. As an example, in this breakout board schematic (here is the link for the product in case someone wants to know where I referenced this schematic from) from sparkfun, you can see two solder jumpers. And this is the picture of how they look on the PCB Solder Jumpers in PCB

\$\endgroup\$
3
\$\begingroup\$

A common way to accomplish what Andy is talking about is to use net ties. They are essentially components that do not end up on the BOM (Bill of Materials) but allow different nets to be tied directly together with copper.

That allows the engineer designing the circuit a bit more control over the layout since the you might want to have all the high current stuff fed off of an separate trace or plane than more sensitive stuff. When the PCB package DRC (design rules check) looks at the copper it will choke because it thinks it sees two different nets shorted together. Altium, for example, has an override that allows net ties specifically to pass DRC.

The other use for this is to enable or disable options, where shunts or switches are not appropriate. Here is one that I'm using today in a design- the circuit will not tolerate the resistance variation of a DIP switch so I have to use a solder short:

enter image description here

The half-moon shape means that a blob of solder will neatly bridge the two sides of the gap.

\$\endgroup\$
3
\$\begingroup\$

When you have several chips all sharing the same supply and you lay out a PCB, you might want to keep the power feeds separate to different parts of the circuit. One way to do this is put links on the PCB. Notice that 3.3V and 3.3VA are basically powered via links from the same regulator - if want to keep them separate on the PCB this makes it easy. If you didn't use links, 3.3V and 3.3VA might get flooded into one plane and cause noise problems.

Notice that AGND is kept separate from the ground around the regulator by doing this too.

I quite often use links on the outputs of switching regulators - this allows me to check that the voltage isn't stupid (due to a fault) before connecting up core voltages on FPGAs - they take some getting off PCBs and I don't like doing it - before using the link, check the voltage is OK then switch off and apply the link. Job done.

\$\endgroup\$

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.