please check the net at design manager on the schematic, if P1 no more connections,  that will not show at PCB.
when you wire the track on P1, you need to update to PCB, or import changes at PCB.
https://docs.easyeda.com/en/Schematic/Convert-to-PCB/index.html#Update-PCB

@tcccorp,

The screenshot you have posted does not show enough of the schematic to see what may be the issue in your project.

• Where do all the nets that are outside the image area connect to?
• Can you make this project public?
• Is it intentional that the pin numbers on your spring terminals that you have labelled "Q1" and "Q2" are duplicated on the upper and lower rows?

@UserSupport

Hello, I made some change, tried to update the PCB and the message is than there is no change

@andyfierman

Hello,  my project is now public . You can see it on https://easyeda.com/tcccorp/save

About spring terminal, yes it is normal because there are 2 pins for 1 contact .

Thanks for your help

@tcccorp,

I'm wondering if the duplicate pin numbers on Q1 and Q2 are causing a problem.

Try creating a new Schematic Symbol for this connector, but this time with only one set of pins numbered 1 to 17. Assign the same PCB footprint to it: that will work fine because a PCB Footprint can have duplicate pin numbers.

Replace the schematic symbols, redraw the connections and try again.

You also need to check the Design Manager (Design button in the left hand panel). In particular, you have a lot of DRC errors in the PCB.

I meant to explain that even if a PCB footprint has multiple pins mapped to the same function as in your Q1 and Q2 connectors, it is normal practice have only one pin on the Schematic Symbol for each unique function. So in the case of Q1 and Q2 you have 17 unique pins on the Schematic Symbol but these are mapped to 17 pairs of pins on the PCB footprint.

Note also that it is not good practice to use the "Q" suffix for parts that are not transistors of some type. The general convention is that the "Q" prefix is used for bipolar transistors (bjts), junction FETs and MOSFETs. MOSFETs sometime use the "M" prefix. "TR" is also sometimes used for transistors.

Connectors are usually "P", "PL", "SKT", "J", "CONN" or something like that.

Hi
Issue confirmed，
That is because of the Q1 and Q2 have the duplicated pin number(two pin1, two pin2 etc), but they connect to different wire.
at present, please use other part instead of Q1 and Q2.
for this issue, we will try to fingure it out before convert to PCB.
Thank you

I have modified this 1X17-SPRINGTERMINAL, please update it at your schematic, and update to PCB.

@tcccorp,

Can you post a link to the datasheet for this 1X17-SPRINGTERMINAL connector?

Thanks.

Are the 17 way connectors made up from stacking these 3 way parts but with only the last one having the end cheek fitted?

So, 5 off 3 way parts with the end cheeks removed and then a 3 way with one way removed but leaving the end cheek in place to make 17 ways?

https://www.adafruit.com/product/1074

https://www.adafruit.com/product/1081

If so then the Schematic Symbol for these connectors does not need to show two pins per way because the two pins are formed from a single conductor and so are internally shorted together. In other words, the Schematic Symbol for a 17 way spring terminal strip needs only 17 pins not 34.

@andyfierman
Andy, Can you help to modify this part, or should I need to remove it?
Thank you

@UserSupport,

I can modify to match this part:

https://www.adafruit.com/product/1074

I will use this datasheet - assuming that the parts are stacked as I described - to check the PCB footprint:

https://cdn-shop.adafruit.com/datasheets/19898.pdf

Note that there is no datasheet for the https://www.adafruit.com/product/1081 part.

Very similar connectors:

https://www.pololu.com/category/175/screwless-terminal-blocks

I'll try to make the side entry footprints compatible for the https://www.adafruit.com/product/1074 parts.

Schematic Symbol and PCB Footprint for:

https://www.adafruit.com/product/1074

Done.

@andyfierman
Many Thanks

@tcccorp,

Please edit your schematic to use the new Schematic Symbol and then do Update PCB... to bring in the new PCB Footprint.

Dear all,

Thanks a lot for your support and sorry for the delay :(

I'm going to check soon as possible !

@tcccorp,

No need to apologise!

If you could verify that I've identified the correct parts and alternatives that would be good.

Thanks.