@usersupport?

You can save as to your personal library and edit it

it's already in my personal library. i created the symbol and footprint. :) the issue is that there doesn't seem to be a way to do a keepout/no solid on ALL layers, not just top and bottom.

@bryan_6020, I haven't had time to check it out in some Gerbers but it looks like you can create a Solid Region, set to "No Solid", and assign it as Multi-Layer within a PCB Footprint in the Footprint Editor: 

Try choosing those two settings; `No Solid` and `Multi-layer`. They're mutually exclusive. EasyEDA won't actually let you select them. @UserSupport, any ideas here?

@bryan_6020, Try this and check the Gerbers in a dummy PCB? In the Footprint Editor, you can set the number of layers in the Layer Manager to the same as those in the PCB that you want to place the footprint on. That then allows you to create a No Solid region on aa Top, Bottom or Inner Layer then copy and paste, or individually draw, it into the other layers.

Last time I checked, it was not possible. However, there is a feature request for this HERE: [Forum - EasyEDA - An Easier Electronic Circuit Design Experience - EasyEDA](https://easyeda.com/forum/topic/Multilayer-Copper-Areas-and-Solid-Regions-38a269596b1a40c2b7d34bedffe4be89)

@bryan_6020, @tobalt, @UserSupport, It's a bit clunky but the process described in my post above works: "In the Footprint Editor, you can set the number of layers in the Layer Manager to the same as those in the PCB that you want to place the footprint on. That then allows you to create a No Solid region on aa Top, Bottom or Inner Layer then copy and paste, or individually draw, it into the other layers." This is a demo footprint:  This is it in a simple PCB with a 4 layer ground flood:  [https://oshwlab.com/andyfierman/demo-of-footprint-with-4-layer-no-solid-regions](https://oshwlab.com/andyfierman/demo-of-footprint-with-4-layer-no-solid-regions)<br> <br> Here's what the Gerbers look like:    

@andyfierman, what happens when you use that four-layer footprint in a two-layer PCB?

@bryan_6020, Sorry, I wrote a description for just that question but it seems to have got lost somewhere... It reverts to Top and Bottom Layer only when placed on a 2 layer PCB. It does not re-revert to 4 layers if a 2 layer PCB on which it has been placed is is then updated to 4 layer. It must be removed and replaced (or maybe Updated from Library?).

Roger. Thanks for that. I'll use this as a workaround for now.

Hi No solid doesn't suuport multilayers, you need to add it for each layer

@UserSupport, For clarity: My posts above show that No Solid can be added for each layer and that it works as expected: 1. In a Footprint; 2. if you create  an N layer Footprint and then place it on an (N-2) layer PCB.

I couldn't actually get that to work. Part is [here](https://easyeda.com/component/89ec4f1c0579404aa482aa232e9317ea). And here's the footprint showing the keepout on one of the inner layers (keepouts are on both inner layers and top and bottom):  and after updating the footprint in a 4-layer board, it still doesn't keep out: 

Have you tried deleting the footprint and then added it back in from that called up in the PCB using Update PCB... ? Have you set the inner layers as planes or signal? I'm not sure what the grey area is where the keep outs should be. Can you share your board or a demo version, with me?

@andyfierman 1) yes. even tried in a new PCB. same issue. 2) they're signals 3) in the photo above, the gray area is a layer in the PCB. it should have no copper there, per the keepouts. 4) done. project is called 'Meadow F7 Core Compute - Developer Module (Dual Ethernet)'. you'll notice in the board that the keepouts work in the top and bottom layers, but not inner 1 and inner 2

@bryan_6020, In the process of trying to understand why your footprint isn't working on your PCB. I have made a little test PCB in your project which shows that it works as expected so now we need to look in more detail to try to discover what it is about your PCB that it doesn't like! Driving back from holiday so probably won't have more time for the next couple of days.

@bryan_6020 Solid Region - No Solid only works for its layer, if you want to every layer no solid, you need to place more no solid at each layer

@usersupport, Sorry but I have already created a public project that shows that when I add a 4 layer Footprint with a no solid on each of the 4 layers, then it works ok. (See my public demo above) I have also shown privately to the OP that his own Footprint  also work in a 4 layer test PCB. I have also shown privately when testing the OPs own PCB thst my 4 layer Footprint with no solids on each layer works in the OPs own PCB. What I have not found is

What I have not found is why the OPs 4 layer footprint with no solids on each layer does not work in the  OPs PCB design.

@UserSupport, Here is my project showing  that when I add a 4 layer Footprint with a no solid on each of the 4 layers into a 4 layer pcb, then it works as intended: [https://oshwlab.com/andyfierman/demo-of-footprint-with-4-layer-no-solid-regions](https://oshwlab.com/andyfierman/demo-of-footprint-with-4-layer-no-solid-regions)

@AndyFierman; thanks for looking. Weird that it works in a new one but no in the one i have.

@bryan_6020, I'll see if I  can find out more in a day or two. :)

In case no one has told you this recently; you're awesome. :)

That's the nicest thing anyone has said to me for a while! If I delete the footprint for U1 in your PCB and then replace it with the MEADOW\_F7V2\_CORE\_COMPUTE footprint from the SHIFT\+F library:  using the same XY co-ordinates then do SHIFT+B to rebuild the copper areas, then I get your PCB but with full 4 layer no-solid regions:  I wonder if the problem may have been that you had not refreshed you library list in between initial footprint pull-in from the Convert to PCB action and when you tried replacing it later. Whereas I opened it in the library with no previous history of it? Odd whatever but it seems to work OK now. So, refresh your library view and then try delete-and-replace followed by SHIFT+B copper area rebuild. I haven't re-run the Design Manager but I think it'll be OK. Let me know what you get?

@bryan_6020, You may have to do Reset Component ID in both the schematic and the PCB after replacing U1 just to stop it being moved outside the PCB next time you do an Update PCB or Import Changes.

Fantastic. It works now. :) thanks!

Yeay! Result!!