One way to do this is to create a pad on `All Layers` with a hole of the specified 2.75mm and a pad diameter of 6.2mm. * Do not assign a net to these pads unless you specifically want them to connect to ground or some other net. That will create copper pads on top and bottom layers which do not connect to anything else and which will also have a clearance around them to any other copper on the board. Another way to do this is to use the hole tool as you have already and then put over it, a `Solid Region` set to `Cutout` and shaped to create the 6.2mm clearance around the hole. This is clunky because you have to manually edit the points of the Solid Region to approximate a round clearance region. See also: https://easyeda.com/forum/topic/Multiples_Inner_board_outline_cut_out-Q5BTN5nFz

Both with the pad and solid region method I end up with cupper/traces floating (solid region leaves the rim). Guess what is really needed is to specify extra clerance around a single component.

`Both with the pad and solid region method I end up with cupper/traces floating (solid region leaves the rim).` Sorry don't understand the issue. If you specify the pad or create the Cutout of the right size then the outer extent of it can be the outer dimension of the required clearance. You still have the copper to copper clearance that is defined in the Design Rules that will give you the required clearance between the screw head, nut or washer. Please see: https://easyeda.com/andyfierman/Holes_with_copper_clearance-b2cf7b27a0934c77858be0b5026d2b2c Can you post a screenshot of what you end up with?

The same as in your example. The outer rim of the solid region is still there. I've indicated it with an arrow: ![enter image description here][1] [1]: /editor/20171117/5a0e0713b5906.png

I don't understand why that is a problem. As I said above, `If you ... create the Cutout of the right size then the outer extent of it can be the outer dimension of the required clearance. You still have the copper to copper clearance that is defined in the Design Rules that will give you the required clearance between the screw head, nut or washer.` The border left by the Cutout defining process does not have to add to the space needed to define the keepout area. Suppose you have a track to track clearance of 0.24mm and you have a keepout around the screw hole to allow for a washer (plus some play) of say 6mm diameter. So, you create the cutout so that the *outside edge* of the border round it is on a diameter of 6mm. Then you have a track-to-outside-edge-of-the-border clearance of 0.25mm.

I've come across this conversation whilst looking for a way to specify no-go areas for tracks prior to running Autoroute or using copper poor. My issue is that the aluminium case into which my board is to be fitted has cast mounting blocks in the bottom which are not round, rather rectangular with rounded corners. I'd like to be able to tell the Autorouter where on the board tracks must NOT go, but so far have been unable to find such a feature. I gues its a kind if extension of design rules. Is there such a feature?

@NuttyProfessor47 Hi, we don't support this feature now, but we will support the keep-out layer in the feature.

@Tutorials Many thanks. As a potential work around, could I lay out the tracks within a "Board Outline" that avoids the No-Go areas, and then change the outline to the actual required board outline afterwards, or would all the tracks re-adjust to the change outline automatically?

@NuttyProfessor47 No, the auto router needs all the components inside the Board Outline,  at now, I suggest that you route it manually.

@NuttyProfessor47, For ground and +5V clearances, you don't need a big copper-free area around the holes. You just need a copper area that is bigger than the mounting pillar dimensions and has a suitable clearance to the surrounding nets and copper areas. Why not just place a circular (or rectangular) 'All Layers' pad with a plated through hole diameter to suit the fixing screw and a pad diameter (or the lengths of the rectangular sides) to suit the pillar dimensions plus some margin for the accumulated tolerances and slop in the screw hole? If you give each of these pads either no netname or maybe give them all a netname of something like 'pillar' then they will not connect to any of the tracks or copper areas but can be accurately positioned and dimensioned.

@andyfierman Thanks Andy. That's what I'll have to do for the fixing holes then. That leaves a pair of other areas that are supposed to be track free, and they are under isolation ICs. I can't seem to copy the diagram, but instead quote from the datasheet for one of them, an AMC1100 - "To maintain the isolation barrier and the common-mode transient immunity (CMTI) of the device, keep the distance between the high-side ground (GND1) and the low-side ground (GND2) at a maximum; that is, _the entire area underneath the device must be kept free of any conducting materials._" As the Autorouter won't run anyway because is says there is only one and it's in use, I suppose the only option for leaving the entire area under an IC free from any conducting material is manual layout. Not quite what I had in mind when I'd read the AutoRouter help, but there you go. In preparation for a manual layout I've been checking the Design Manager Nets and Connections, and seem to have aquired a number of "Nets" of the form S$number. Selecting any of them doesn't highlight any Ratlines on the layout, so what are they? Spice suedo nets perchance that can safely be ignored?

"...That leaves a pair of other areas that are supposed to be track free, and they are under isolation ICs...." You could do the same trick using a pad. Place a rectangular pad in the area you want to keep tracks and copper out of then leave the netname blank. The router should route round them. Then when you're done, delete them. Beware though that the copper flood may still then fill the are if it auto-rebuilds the Copper Areas. You may need to manually craft the copper areas around these regions to stop that happening. A better solution is as I have described above using the **Solid Region** tool to create a cutout. Even though the cutout region is shown as having an outline, this is a PCB editor visualisation aid: in the Gerber output, that outline does not exist, only the cutout region remains. You can of course use this for the pillars too but the downside is that Solid Regions are not so easy to create and position as pads. "...seem to have aquired a number of "Nets" of the form S$number..." Check for orphaned short traces (or traces with a length equal to the trace width that just look like a dot). These can sometimes be left over from trace editing. If you click on them in the Design Manager and they then show up as being connected to pins in the lower part of the DM panel, click on the pins and a highlighter should point to the pins to help you located them. Sometimes, the silkscreen outlines and other drawing elements can be assigned S$ net numbers in which case you can ignore them. Click on the tick next to it in the DM and see what toggles in the PCB view.

If it is not too late, I found a solution: \- Make circle \- right\-click \- convert to Solid Region \- Move to Layer with copper you want cutout on \- Set type to \- No Solid \- Rebuild copper

@jhuljev Brilliant, thank you