Hi Ken, There are a couple of ways to do this. To make an **unplated circular hole**, you can use the `Hole` tool button on the PCB Tools floating palette. To make a **plated though circular hole** you can use the `Pad` button on the PCB Tools floating palette. Just set the`Hole` parameter to the diameter you require for the mounting posts. So, for example, make the hole diameter to 3.5mm for M3 clearance holes. Note that, using this tool though you can only make plated through holes because you cannot set the pad diameter to be the same as the hole diameter. Using this tool, you are also advised to create a schematic symbol for the pad and place that in the schematic first. If you do not do this then, after placing the pad into the PCB layout, the next time you do **Import Changes* into the PCB layout then the pads will be deleted!

IT IS MORE THAN A "HOLE" . . . . A CUTOUT FROM THE BOARD EDGE 9mm X 6mm

Is this a hole within, i.e. enclosed by, the PCB or is this just essentially an irregular board outline?

i WOULD SAY THIS IS THE LATER . . "IRREGULAR BOARD OUTLINE".

How to create a hole of an arbitrary shape enclosed within the PCB is described in the later part of: https://easyeda.com/Doc/Tutorial/PCB.htm#Solid-Region-in-PCB To create an irregular board outline then you can simply draw it on the **Board Ouline** layer using the `Track` button on the PCB Tools floating palette.

BTW: Double clicking on a segment of a selected Track between the green and blue dots (on any layer including board outline) splits the clicked-on segment into two to help in moving segments around. Double clicking on a green dot on a segment, deletes it.

![enter image description here][1] [1]: /editor/20160207/56b67a582164e.png

This is what I am trying to accomplish . . . I don't get the instructions . . . please help. Thanks, Ken

But Ken, accorcing to that screenshot you have already accomplished it! If the purple (or magenta depending on exactly how your monitor renders it) outline shown in the screenshot you have just posted was drawn in the `Board Outline` layer of the PCB, then that outline ***is*** the board outline that the PCB will be made to. You don't need to do anything else. Here's a screenshot of another example of an irregular PCB ouline, showing the layers dialogue panel: ![enter image description here][1] [1]: /editor/20160207/56b68a9bf22c1.png

You do need to make sure that the board outline is closed i.e. all the start and end points of lines and arcs lie exactly on top of each other. If you have drawn an arc and then copied, pasted and rotated it to save redrawing it, that can sometimes generate `Board Outline not closed` error warnings. We haven't got to the bottom of why that can sometimes happen and if it does then you will have to draw each arc in the right orientation as you require it.

Ok, I corrected the paste & rotate arc and reviewed the end points and still get the error! I also removed the arcs and closed with a straight track and got the error.

hi, you can use solid regin to do cut out. If you can not get rid of, please share it to Andyfierman@easyeda.com private.

Ken, Another tip is to use the coarsest `snap size` you can when you draw the outline. The finer the grid, the harder it is to ensure that the end points are exactly superimposed. If you still get the error, try drawing the whole outline, including the indent sections but omitting the arcs (drawn to create the semicircles) as two separate sections: the top piece and the bottom piece. Draw both on a coarse grid and then move them to where you want them. Lastly draw the two semicircles on whatever `snap size` you need to get the right shape and to get the end points in the right place on grid then reset the `snap size` back to coarse to align them with the end points of the indented sections. For example, with your outline, if you set the `snap size` to the same as the `Grid` you can draw everything and the end points can be snapped to exactly align. Does that work? One other thing to check. If you make the `Board Outline` the only active layer and then do `Fit in Window`, does the outline then fill the whole window (as far as the aspect ratio allows of course)? If not then you have something else in the `Board Outline` layer that is not showing up. That will cause a `Board outline not closed` error so it needs to be deleted. It could be a zero length line which will be hard to find so it may just be easier to do `CTRL+A`, then `DEL` and draw it again from scratch.

Ok, Got it! Thanks for your help :) Ken