Can you post the url of a public copy of your project please?

@andyfierman Thanks.  Can you see this ? [Nixie display board](https://easyeda.com/netdudeuk/nixie-display-board_copy_copy)

@netdudeuk Hello Looks like you have misunderstand the footprint package that you used for the Nixie model that you have dropped in your schematic. Regarding the Schematic, your pin number 1 is connected to the resistor YES BUT regarding the module footprint it looks like pin 1 in the Schematic is set to pin 5 in the footprint package. Check the following images and make a check on your components footprints and you will find that there is a mistake in the component "pin number"  Here is your component connected to the resistor, it's true BUT the following image is related to the footprint and it shows that pin 1 of the schematic is pin 5 in the PCB  Please review each uploaded component before using it directly, especially the footprints :) Nice design by the way

@netdudeuk, Can you identify exactly which Schematic Symbol and which PCB Foot[print that you have used in your project? A screenshot of where you find it using the SHIFT+F search libraries tool would be best or the url of the component if you search in the general site search tool.

@andyfierman The footprint is as follows : DISP\_IN\-12\_SOCKET And here is a screenshot of where you can get it from the library :  The Footprint order of the PCB lib is not matching the pin numbers order in the schematic lib **Schematic pin      PCB pin** - - - Pin1                     Pin5 Pin2                     Pin4 Pin3                     Pin3 Pin4                     Pin2 Pin5                     Pin1 Pin6                     Pin12 Pin7                     Pin11 Pin8                     Pin10 Pin9                     Pin9 Pin10                   Pin8 Pin11                   Pin7 Pin12                   Pin6 - - - So the user has followed the schematic pin order to wire the PCB pads which leads to the fault.

@JLCPCBsupport, If you are sure that @netdudeuk has used that particular Schematic Symbol and PCB footprint then there are a number of issues that have lead to what has gone wrong with this PCB and which need to be addressed. 1) It would appear that the Design Flow in the main Tutorial and the essential checklists (4) and (6) in (2) in: [https://easyeda.com/forum/topic/Big-PCB-fail-nets-don-t-match-schematic-fd1741fd83a74f80854f08b18ca00045](https://easyeda.com/forum/topic/Big-PCB-fail-nets-don-t-match-schematic-fd1741fd83a74f80854f08b18ca00045) have not been followed. If the Design Flow and checklists had been followed then the mismatch in the Schematic Symbol pin to PCB Footprint pad mapping would have been identified before submitting the PCB for manufacture. It is the designer's responsibility to do this. 2) The advice that is issued at the foot of the PCB order page: [https://cart.jlcpcb.com/?fileId=b480258ce7bb48cba9a347f007a91715&uuid=48ad4c94440d419da88d264b25b72e41&achieveDate=72&eadLink=2&electropolishingOnlyNo=no](https://cart.jlcpcb.com/?fileId=b480258ce7bb48cba9a347f007a91715&uuid=48ad4c94440d419da88d264b25b72e41&achieveDate=72&eadLink=2&electropolishingOnlyNo=no)  has not been followed carefully enough particularly with regard to section 13 in the linked [instructions for ordering](https://support.jlcpcb.com/article/68-instructions-for-ordering?_ga=2.26574142.2074837760.1595153418-139248169.1592496815) document: [https://support.jlcpcb.com/article/68-instructions-for-ordering?_ga=2.26574142.2074837760.1595153418-139248169.1592496815](https://support.jlcpcb.com/article/68-instructions-for-ordering?_ga=2.26574142.2074837760.1595153418-139248169.1592496815) **13\. About file generated from Easyeda** Easyeda is a free online tool that we provide to design the PCB, and you can place your order on JLCPCB easily and quickly.  But if there is manufacturer error due to the design error, we may not responsible for that. It is the designer's responsibility to do this. 3) The Schematic Symbol and PCB Footprint was orginally from Dangerous Prototypes and appears to have been copied without being checked before adding to the EasyEDA System library. I believe that this is a mistake because there is a comment from 2014 on the Dangerous Prototypes blog that warns that the pin mapping in wrong! [http://dangerousprototypes.com/blog/2012/09/11/eagle-parts-in-12-nixie-and-iv-22-vfd-tubes/](http://dangerousprototypes.com/blog/2012/09/11/eagle-parts-in-12-nixie-and-iv-22-vfd-tubes/) 4) It is not clear if anyone has submitted an error report about the pin mapping mistake to get the library footprint corrected.

@andyfierman @JLCPCBsuppor Yes, that is indeed the one. I believe that Dangerous Prototypes are a well established and reputable brand so I didn't think that I needed to check their submission.  I sent them a message yesterday. I wasn't looking for JLPCB to make things right.  I've actually managed to do this by putting the tubes on the reverse side of the PCB, where they actually look better.  I just need to swap two of the digits in my code as K6 and K8 are still interchanged. Thanks both for your help with this.  It's been a really good learning exercise to start off with a blank canvas, create a schematic, turn that into a PCB layout, upload it to JLPCB and get some professional grade PCBs for a really good price.  I'm looking for my next opportunity to do so. I had a quick look at Kicad yesterday.  It would be great if EasyEDA ran the tracks around IC pads, etc. when laying them down, just like Kicad does.  It would make manual routing so much easier. Thanks again.

@netdudeuk, I am glad that you have been able to work around a a problem that I consider to be an oversight on the part of EasyEDA in creating library parts. :) Doh, sorry. I just spotted a copy and paste error in my previous post. It should have referred you to: "... the Design Flow in the main Tutorial and the essential checklists (4) and (6) in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) I know it's a lot of reading but it really does save a huge amount of hassle if you can set aside the time to read the above document and all the further documents that it links to. It should make your next project run a lot smoother and make it more fun along the way. On the subject of: "It would be great if EasyEDA ran the tracks around IC pads, etc. when laying them down, just like Kicad does." If you are referring to Kicad's "Push-and-shove" routing feature then you might like to +1 this topic: [https://easyeda.com/forum/topic/Push-Shove-Routing-d936ed98a0ce4895978eb9dc17242963](https://easyeda.com/forum/topic/Push-Shove-Routing-d936ed98a0ce4895978eb9dc17242963)

@netdudeuk You are welcome As I mentioned already, check the components before moving to production and you will be safe. This is a mistake to learn from it so keep going and good luck :)

@andyfierman @JLCPCBsupport Thanks folks. Check it out ;-) [IN-12A Nixie tube on JLPCB board](https://youtu.be/lFXkABQor1o) That's obviously just one portion of the board populated but that's with no bodges. As it happens, I didn't even need to mess with the code.  Every digit works as it should.  I'm very pleased with the PCB and the service from JLPCB.  I really liked watching it go through the different processes and seeing it shipped in no time at all.