RJ45 will not connect

In schematic, I have several RJ45 connectors. Some of the LED pins are connected to resistors. I found a shielded connector in the footprint assignment. Now I am in PCB and pins 9, 10, 11, 12 are renamed GK, GA, YK, YA. Some of these pins are connected to resistors but the resistor leg and the RJ45 pin are in large font and there is no net line tying them together. Why are they not showing a connection in PCB but in schematic, they are connected? How do I fix this?

  1. Read the FAQ article, How does KiCad know which symbol pin represents which pad of the footprint? .

  2. Edit either the symbol, or the footprint, until they meet the requirements explained in the above article. The following FAQ articles may be helpful:
    Tutorial: How to make a symbol
    Tutorial: How to make a footprint (From scratch)?

  3. Save the modified items (footprint and/or symbol) and use the modified version(s) in your project.



Thank you very much. Now, I can get back to building another board while watching a bad movie.

Where did you get your RJ45 footprint from? Most of the RJ45 footprints in the standard libraries use pins 9, 10, 11, and 12 for the LED pins.

What is the exact footprint name (cut and paste from your schematic symbol)? What is the part number of the connector you plan on using? You should double (and maybe triple) check that the footprint you are using mechanically matches the datasheet drawing of the connector you plan on using. There is no such thing as a “standard” footprint for pretty much any connector. The electrical pins might be the same but the quantity, location, and size of mounting hardware is usually specific to the connector being used. Even more so when adding in accessory pins like the LED pins.


This reminds me of the LM7805 issue a couple of years ago, where the schematic symbol used pin names rather than numbers

That was before @jkriege2 took on the massive job of reworking the regulator lib. (Checking this massive change was one of my first tasks as an official maintainer. Which means this must be more than a few years ago.)

1 Like

I am currently using a generic footprint from the list(connectors: RJ45_TRANSFO). I ordered a box of RJ45 connectors. When they arrive, I will check part number and look for datasheet drawing. I will also transfer to AutoCad and print it 1 to 1. I will then make a visual comparison. I usually make sure I have all parts and that they fit the paper before I press the order for the board. With other SMD type components, it is easy to test. I will also check polarity of the LEDs.

A couple points:

  • First, by the library name that looks like it is from pre-v5 libraries.
    • One of the reorganization things that was done to the libraries for v5 was to remove the plural “s” from the library name. I’m sorry to say that I no longer have the pre-v5 libraries installed so I can’t look at it myself. In the v5 libraries the RJ connector footprints are in the library named Connector_RJ, and there isn’t a “generic” footprint in that library for the reasons I explained before. Each footprint is designed for a specific connector as indicated in the footprint name. But, there might be one of them that is close enough to directly fit or just need a little tweaking to fit your connector.
    • What version of KiCad are you using? If you are on v5 and still have v4 libraries, check out these FAQ entries, I had KiCad 4 installed previosly. Now i updated to v5. Now i have some problems with the library setup and Converting KiCad version 4 projects to version 5 (Remap a project). IMHO incorporating the new library organization will get you to better constructed symbols and footprints.
    • If you aren’t on v5 yet, are you at a good place in your projects to spend the time to upgrade? That will help you get better support here as most of us have already upgraded and don’t have access to pre v5 to test things out.
  • Second, then footprint name RJ45_TRANSFO makes me wonder if you selected the correct footprint to start with. Are you using Ethernet signalling, or just using LAN cables as a simple to use 8-conductor or 4-pair cable?
    • This footprint was probably (based on the name) designed for an RJ45 connector with an integrated transformer (also referred to as integrated magnetics), specifically for Ethernet signalling providing isolation from the rest of the network. (See this discussion if you aren’t sure what I mean. I original though it was for PoE until I did a little research for this answer… Thanx for the opportunity to learn something new.) Because of the integrated transformer they are usually larger than a simple RJ-45 connector, and are wired up completely differently. This means you don’t have to put a LAN transformer on your PCB (it’s already integrated into the connector), but it also means that you can’t use the RJ-45 connector for anything else other than Ethernet (or similar high speed signalling using the same conductors on the cable as Ethernet).
    • If you want to just use the RJ jack as a simple cable you can’t use the transformer version because you will not have direct electrical connection to each and every wire of the cable.

Just trying to make sure you don’t fall into a hidden trap.

1 Like

Thanks a bunch for the learning opportunity and helping me avoid a hidden trap. I had the previous version of my FPGA board system with the green screw terminal type connectors. They are ugly and confusing. I then went to a recycle center and purchased a few cubic feet of (soft and stranded) CAT5 and CAT6 cable in lengths of 6 and 10 feet and in pretty colors. I have a commercial version of the RJ45 crimper so I put 2 and 2 together. I purchased the non transformer type. They arrived today and are straight through. I did not know about the transformer in the longer types but I did wonder why they were longer. For once blind luck is on my side. After much testing, the next version of my PCB board will have 5-RJ45 connectors. I hate those DIN things. The RJ45s will not be paired for Ethernet but will be paired for GPIO to ground, for servos, and multi power to drive opamps, etc. I did not see the reason for keyed connectors. After they are tagged and connected and tested, I will use a zip tie on each to avoid a casual disconnect and mis-connect. All connectors will use the common twisted pair configuration used in Ethernet. My present board does everything I need and this next ver. RJ45 board will be much cleaner. Also doing without the DIN connectors, my cabinet volume will be reduced as well as cabinet cost.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.