I'm not sure from your post but if you want the pads to **not** have exposed copper then apply a negative soldermask offset to the pads of at least half the track width. That will close the solder mask aperture over all the pads. Check the Footprint by placing it in a simple test PCB and then generating, downloading and checking the Gerbers using gerbv as recommended in the Tutorial. Do not rely on the JLCPCB gerber tools for checking.

Thank you for your answer Andy. I'm having troubles installing gerbv, but I viewed the Gerbers using [http://mayhewlabs.com/webGerber/](http://mayhewlabs.com/webGerber/). It confirmed the problem visible on the 2D view of EasyEDA. I'm OK with the pads being exposed (that's on purpose), but the problem I have is that the solder mask aperture expands down to the center of this circular zone. I updated the project with a copper area to better demonstrate the problem (see picture attached). The copper area in the middle of the footprint gets exposed, which I would like to avoid.  

In the image above, there appears to be a copper area in the middle of the Footprint. If that is the case then it must be is a separate pad from the concentric structures so you can select that and apply a negative soldermask offset of at least the radius of that pad. However, your Footprint shown in: [https://easyeda.com/bencfd/exposed-copper](https://easyeda.com/bencfd/exposed-copper)<br> <br> has no centre pad. Can you post the url of the Footprint rather than the PCB you have placed it on?

Indeed, there is a copper area in the middle of the footprint, ie inside the circular pads converted from tracks. It is built with _Copper Area Manager_, not from a pad, but it strangely gets exposed. Here is a link to the footprint, I hope it helps. [https://easyeda.com/component/52a7d0a0ad1c44bd9c4c0c06eaba7de2](https://easyeda.com/component/52a7d0a0ad1c44bd9c4c0c06eaba7de2) Thank you for your help!

This topic: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6)<br> <br> advises making **all** copper elements in a Footprint out of pads. If you modify the Footprint to make the inner circle of copper out of a pad then do the negative solder mask offset to cover it, that should do what you want. It will also create a Footprint that shows all its elements both in the Footprint Editor and when placed.

I effectively followed this topic's advice and made all elements of the footprint out of pads. But I managed to isolate the problem. It comes from the outer circular pad. When it's about to close down to an entire circle, and when the (Top)SolderMaskLayer of the two tips of the arc overlay on one another, then the copper area gets exposed (**top** on the below figure; design is captured without showing the board's copper area). With more distance between the two tips of the pad, the copper area is not exposed (**bottom**). :) 

OK, I understand how you've got the central copper now. Your work around seems reasonable but I think a centre pad with a closed off solder mask might be a safer option if you always want copper in the centre. It's a bit strange that closing the arc causes this issue (I think I have seen this before but cannot recall which topic...) but it's probably more of a "feature" than a bug worth reporting. BTW, did you find George Lepple's OS X packaged version of gerbv from here? [http://gerbv.geda-project.org/](http://gerbv.geda-project.org/)<br> <br> :)

I tried a centre pad with a negative solder mask expansion, it works, yes, but I prefer to avoid this design because I want to place another component's pads in this area. I've found the package version of gerbv by Lepple, yes, but it requires fink, and it is not yet available for macOS 11. I registered to the mailing list to be informed when it will be available. ;)

I edited the topic's title to mark it as solved. Thank you again for your help!