Can you make your project public?

Hi yes of course
thanks in advanced

To ensure that I have reviewed your project at - or as near as possible - to the time when you made it public and not after you may have made any changes to it, I have taken a copy of:

https://easyeda.com/pjtechgroup/provaas_recover

and have reviewed that as at 200329:

https://easyeda.com/andyfierman/anf-copy-of-provaas

**Schematic: **

The following is my review of your project at that point. It comprises three sections: Schematic, PCB and Conclusions.

1) Your schematic is drawn badly.

Every wire overhangs the symbol pin to which it is intended to be attached.

This makes it unnecessarily hard to read:

This is expressly identified as bad practice in the checklist (4) in (2) in:

https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a

2. Except for the +12V and GND nets, you have not applied net labels to any of the nets which is recommended in the checklist (4) to help identify nets in both the schematic and the PCB and to help identify connectivity errors.

3. It is good practice to apply Not Connected crosses to unconnected pins:

This is also in the check list in (4):

4. It is not good practice to join more than two wires at the same point as you have done at the 12V net at SW3 pin 2.

This is also in the check list in (4):

PCB

5. Your PCB layout makes it very difficult to efficiently route between the transistor collectors to the switches, the resistors and then the LEDs:

Unless you are committed to this layout (you have not uploaded a Design Requirement Spec so I can't tell), I suggest you rearrange the layout so that the nets flow more around the board. I would suggest putting the transistors so that their collectors are close to the switches and then the resistors flowing from the other side of the switches to the leds. If you use larger resistors you can get traces between the pads more easily to help ease routing bottlenecks. See point 6 below.

6. The PCB Footprint, RES-SMD_L1.2-W0.6, that is associated with your resistor R1 & R7, LCSC p/n C136993 (NOTE it is not C136993 as in your LCSC p/n attribute in the schematic) is not correct for the 2512 package size of the component. You must check all symbols and footprints against the datasheet as as described in the checklist (4) and (6) in (2) in:

https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a

7. If you make these changes, you should find that you do not need to go to the huge expense of an 8 layer PCB! (Actually I think it can be done on 2 layers, ;) )

8. Please do not expect too much of the EasyEDA Autorouter: it is far from optimal. With some thinking through, trying out a few different layouts and a bit of practice, you should be able to route a PCB like this by hand.