"the v-cut annotations appeared on the same Board Outline layer (I read that this needs to be on the Mechanical Layer)." To be absolutely clear: V-Cut lines must be on and only on the Board Outline Layer. Somewhere, long, long ago in a topic far, far away there was a post about this to correct a misstatement on the JLCPCB pages but that is now lost beyond the reach of the EasyEDA search tools... :)

@ElliotFan, * It would be helpful to change the colour of the Mechanical layer so that it is clearly different from that of the Board Outline layer. * Whilst reading (2.2) 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)<br> <br> you will have seen a statement along the lines of: "If it's on - or forms an integral part of - the PCB then it must be represented in the schematic". Put two single pin headers in the schematic and assign footprints to them for multilayer (through hole) pads with hole diameters suitable for the wire size that you intend to use to wire these units together. Set the **Add to BOM** attribute for the headers to **No**. Set the **Convert to PCB** attribute for the headers to **Yes**. Hint: if it is the right size, reproduce the pad you have already used in the Footprint Editor and save it with a unique name then assign that to your headers in the schematic. Then do update PCB. * There is insufficient spacing between the panels for the V-Cut lines: they will rip the edges of the pads: [https://jlcpcb.com/capabilities/Capabilities](https://jlcpcb.com/capabilities/Capabilities) > Board Outlines > Trace to V-cut line * Not sure why you have added copper flood top and bottom as the board size is so small it will do little to act as a heatsink. Since the part you have chosen is specified to supply a constant 15mA you can use single sided copper tracks. A width of from about 1mm up to the device pad width would be OK.  * Note that the power dissipation will increase linearly with the voltage drop across the device\. For example\, it you're supplying a series string of 10 LEDs each with a forward drop of 3\.5V @ 15mA from a supply of 40V then there will be 5V across the regulator giving a power dissipation in it of \(40\-35\)V\*15mA = 75mW\. If your supply increases to 60V then that power dissipation goes up to \(60\-35\)V\*15mA = 375mW\. * Check the Package Thermal Data, the notes associated with it on page 4 and the section on Power Dissipation on pages 8 & 9 in: [https://www.diodes.com/assets/Datasheets/AL5809.pdf](https://www.diodes.com/assets/Datasheets/AL5809.pdf) * Check out the User Guide: [https://www.diodes.com/assets/Evaluation-Boards/AL5809EV1XXXUserGuide.pdf](https://www.diodes.com/assets/Evaluation-Boards/AL5809EV1XXXUserGuide.pdf)<br> <br>

@andyfierman Thanks for your detailed comments, very helpful! Your comment about adding two single pin headers... If I understood correctly, is this to address my in/out contact points on either end of the board which have no representation in the schematic (since easyEDA doesn't provide means for adding stand-alone pads in schematic)? The board's intended application will only see fairly low voltage drops across the regulator, ie less than 90mW dissipation.

"...easyEDA doesn't provide means for adding stand-alone pads in schematic" Yes it does in exactly the way I described. :)

@andyfierman Hah! we are talking in circles! got it, thanks. Based on what I read on Panelize: [https://docs.easyeda.com/en/PCB/Panelize/index.html](https://docs.easyeda.com/en/PCB/Panelize/index.html) looks like JLCPCB already knows to expand the pcb design/components to the all the panels even though the Panelize function only panelizes the board outline. I noticed the BOM file lists quantities for only the initial panel. Does JLCPCB automatically multiply the quantities by the number of panelized panels?  This would also affect the cost quote. I did see that others have asked about this issue (about 2 years ago) but I did not see any clear answer.

I've not used Panelisation so I can't give a definitive answer about copying across the panels and the subsequent component quantities. You could try a dummy run through the ordering tool to order your boards stopping before payment, setting the panelisation option and see what it comes back with in costs and component quantities The best thing to do is to post a question just about that including your own panelised screenshots in the JLCPCB Category.