Hi, This is a big project, I think you have spent lots of time on this project. Hope EasyEDA's users can buy your product and support you. EasyEDA will buy one if you like to sell. I need some time to answer your question, please wait for some time.

@Braedon, If the board outlines are not simple rectangles then you need to separate them by at least 2mm. This is to allow room for the V cutter head to turn as it follows the line of the edge. If they are simple rectangles then the board outlines can overlap but you must allow for the fact that the V-cut effectively reduces the surface area with respect to the centre line of the cut so it would be wise to make sure that all components and copper are clear of any section of the board outline that is to be V-cut by at least (1mm + 0.5*the board thickness). This is because the edges of a V-cut PCB are not perpendicular as they are on an ordinary, single PCB. The picture below illustrates these dimensions. ![enter image description here][1] [1]: /editor/20160622/576a41feca044.png

@Andyfierman , Braedon's PCB no way to v-cut. because the v-cut just support straight line and can't stop, must start from one side to another side. And I think Braedon don't need to v-cut. Your only problem is that you can use't copper area, because EasyEDA's copper area does not support the a board outline in a board outline. Check the bellow image. If you need to use copper area and want to draw a hole like left, not OK, but right is OK . ![enter image description here][1] If you don't need the copper area, you can delete all of your copper area and keep to design, your PCB not problem to fabricate, EasyEDA or some other PCB houses can help you to cut the PCB to small PCBs. But if you need to use copper area in EasyEDA, there is a way. change the red arrows board outline to silk layer, when you order, you must told the EasyEDA or other PCB house that you need to cut. That is All. This is not design problem, just EasyEDA's copper area algorithm needs to improve. ![enter image description here][2] At here, I answer what is zero and 2mm to penalized. the red arrow can use v-cut(line, just like a knife to draw a line), the green arrow should be cut.( 2mm at least). keep this in mind, if need a space, the space must be 2mm+, or no space(zero). For the `dose` to `does`, will be fixed next version, a few days later, but will keep SolidRegion , I think this is a key words, :). ![enter image description here][3] [1]: /editor/20160622/576a459374fa4.png [2]: /editor/20160622/576a49d95f612.png [3]: /editor/20160622/576a48b6239b2.png

I was having trouble getting the remaining copper areas to be solid after doing the 2 large areas. It was going to be a question for another post once I'd sorted the board cutting out. So If I read your last comment correctly, if I replace all the internal board outlines with silk layer lines, and when ordering say that I want to cut along those lines (ie I give them labels on the silk layer) that will be the minimum required due to the irregular shape of the outline at the bottom and top left corner making cutting Vs difficult to automate as the software is written at this time. There is another PCB simillarly named but with route-cut at the end of the name here -> https://easyeda.com/editor#id=FiE0mI4pn I was having issues getting some of the copper areas to go solid, but the original idea was to route out the area between the boards and then dremel out the small joins I left in the PCB. The solid areas were a real issue though, but as you hinted, the algorithm might not be up to it unless I make one huge copper area that covers the whole thing, but then I get bare copper under the solder mask where I cut out the joins (unless I put a copper cut out area over them?). Then I also get my rounded corners... The whole thing is just a part of my fully self contained electronics test bench for testing components, power distribution, and Arduino programming (via USB or hopefully Bluetooth). It all sits on a portable panel of MDF with an ATX Powersupply modified as a benchtop power supply that feeds into the lower middle panel. That way I can go anywhere in the house or the back veranda where there is 240V and breadboard and test in peace... This is v0.1. I could make it simpler, or do it with individual devices for each function, but that would take up more room and not be as portable. Thus I'm trying not to make it too expensive to fabricate.

>I was having trouble getting the remaining copper areas to be solid after doing the 2 large areas Because the board outline is cross, not a Closed curve. and https://easyeda.com/editor#id=FiE0mI4pn this version is OK, and no inner board outline, so you can use it as copper area. but I think you use silk layer and and give some note to order, every PCB house can help you to this. There is hack way to create a inner board outline: you create create a very thin NPTH solid region, make it looks like a line. NPTH will be export to board outline too. All of your round corners no problems, I don't know what you worry about. Your Project is very interested. We hope we can help you to sell to our EasyEDA users.

OK, I will go back to that version then. What is the minimum width of an NPTH. I presume you need to allow some minimum width for a router or tool of some sort to make the hole (??). Thanks again for all your help guys. cheers Braedon

Assuming I didn't make it zero like the hack of course, and wanted it as a real rectangular or other shaped hole.

Also, I just noticed that your quoted maximum board size specs are 300x300mm, my PCB is nearly 400mm wide. Will I have to modify this? Also I have some 10mm drill holes that I'll need to turn into NPTHs to meet the maximum 6.25mm in your manufacturing specs. I take it the order process doesn't check for errors like the size being too large or holes being out of spec as nothing has flagged the issue when I check the order page to see how much the different board areas I have tried affected the cost.

I created a copy here -> https://easyeda.com/editor#id=OvHFfdbwu I put copper region cutouts over the joins between the sub-boards so that when cut there is no exposed copper at the edges under the mask when cut, and silk layer lines to indicate where to cut. I'll make the NPTH areas narrower for the final version (thus the question of minimum NPTH tool width). if I have the "keep island" property enabled on teh copper areas, I don't have to leave a tiny sliver of copper on some joins so that the copper fill area algorithm would fill the areas blocked by the solid region cutouts. It obviously uses an algorithm similar to the "Fill" area algorythm in Photoshop where it looks for adjacent space inside the board outline. cheers Braedon

> an NPTH. I presume you need to allow some minimum width for a router or tool of some sort to make the hole I think this is price problem, for good price, you need to keep 2mm, we can do 0.6mm, but the price will be higher. > 300x300mm, my PCB is nearly 400mm wide Sorry, we forget to change, support 450mm for good price, so your PCB is OK. we even can do 1000mm >Also I have some 10mm drill holes 6.5mm mean round hole for round drill, more than that size, we will help you to cut the hole, the hole should be almost round. No need to add the cost. Your new copy is OK. When you place the order, you must choose, because you try to penalized lots of different PCB on the same PCB. Your PCB is 7 small PCBs, at present, if more than 5, we don't change any more, will give 2 as free. ![enter image description here][1] [1]: /editor/20160623/576b32615779e.png

Ah. I thought that option was for the same PCB repeated over and over?

Hi, If you need to repeated over and over, you don't need to choose, you can ask us to help you to repeat. Such AS 3X3 , it will be bellow image ![enter image description here][1] [1]: /editor/20160623/576b50aeb6e94.png

It's OK, I don't need that, I just thought that's what the option was for, that's all. The 10cm holes are all perfectly round so no issue there, and I'll make sure all the NPTHs are at least 2mm wide. cheers Braedon

I found a neat workaround to the issue of multiple copper areas that don't fill. A single isolated via without any connected tracks on the same net as the copper area, somewhere on the copper area causes it to fill. I now seem to be able to put as many disconnected copper areas in as many different nets as I want on the same PCB, where before I could only put 2 per side (of 2 layer board). Cheers Braedon

Are you saying that if you have say 3 isolated copper areas and you give them all the same netlabel, for example, `COPPERNET`, and if you put a via into each of the three areas and also netlabel the via `COPPERNET` then you can place all three copper areas and they fill properly? Have you checked the Design Manager for net and pin errors after you have done this? :)

Different net labels per copper area (other than front and back connected with the Via), but yes, that is correct. That is with keep islands off too. I've not checked it in design manager, no. https://easyeda.com/editor#id=OvHFfdbwu cheers Braedon

Do you mind to add an image and mark where is the problem, btw, your PCB is private, I can't check.