A copper area used for a capacitive touch contact must be covered by Solder Mask and therefore also does not require a Paste Mask aperture. The recommended process in EasyEDA for anything that is on or forms an integral part of the PCB is to: 1. first create and save a named PCB Footprint and then 2. to create and save a Schematic symbol with the same name and having the named PCB Footprint assigned to the Package attribute of the symbol. The problem is that if a PCB Footprint for such a contact is made using the Solid Region tool to define the copper area then attempting to route a track to it will cause DRC errors when it is pulled into in a PCB from it's associated Schematic Symbol. This is because a Solid Region can not be assigned a pad number. The recommended EasyEDA procedure for creating _anything_ copper in a PCB Footprint it to use only Pads. A Solid Region can be converted to a pad, which solves the pad number assignment problem but the problem then is that copper over Pads is automatically assigned an aperture in the Solder Mask and Paste Mask layers over it. * However, there is a way to remove these apertures over a pad. **Since the update to EasyEDA V6.2 it is possible to set a _negative_ Solder and Paste Mask expansion.** A positive expansion increases the radius or width/height of the aperture. A negative expansion reduces the radius or width/height of the aperture. For circular pads of diameter D, the expansion must be equal to at least -D/2. For rectangular pads the negative expansion only needs to be at least half of the smallest dimension. Irregularly shaped pads may require some experimentation to reduce the aperture to zero. It is possible to set a negative expansion of greater than that required to reduce the aperture to zero For example, a circular pad with a 60mil diameter then specifying a SolderMask and a PasteMask expansion of -30mil for both apertures will reduce the aperture to zero. **Covered pads created this way must be checked by generating and inspecting them in Gerber form using gerbv.**