In EasyEDA, vias they are covered with solder mask by default. Multiple vias can be used to reduce the electrical or thermal resistance between one section of track or a copper area to another on a different layer on a PCB without exposing any copper. To avoid DRC errors in a PCB Footprint, it is recommended to use pads and not vias. Pads by definition are intended to be areas of exposed copper and therefore by default are not covered in solder mask. There are times when it is required to make a through hole connection between pads in a PCB Footprint but which may require that one or both sides of the pad be covered by solder mask. This topic describes a way to achieve this. The following creates a footprint with a top layer of exposed copper and a paste mask aperture created for it, a number of through hole pads with the top layer exposed but the bottom layer covered in solder mask and a bottom layer pad that is covered in solder mask and does not have any paste mask aperture created for it. 1. Place a Top Layer pad defining the area to be thermally or electrically enhanced. This pad will be exposed copper; 2. Set this pad to the required number. For example, N. 3. Place a through hole pad of the required hole and pad diameters into the Top Layer pad; 4. Set this pad to be number N. 5. Set the Solder Mask Expansion to the smallest dimension of the pad multiplied by at least -0.55 (if the pad is round then this is -0.55 times the radius, if it is oval or rectangular then this is -0.55 times the smaller dimension. For example if the pad is 2mm diameter then set the Solder Mask Expansion to -1.1.mm. The factor of 0.55 is to avoid the possibility of leaving a tiny hole due to rounding errors when swapping between metric and imperial units). This closes the Solder mask over both sides of the through hole pad; 6. Copy and paste this pad into the Top Layer pad, arranging them as required; 7. Ensure that they are all set to pad number N; 8. Copy and paste the Top Layer pad onto the bottom layer (Or create a new Bottom Layer only pad of the required shape); 9. Ensure that this Bottom Layer pad is numbered as pad number N; 10. Set the Solder Mask Expansion for this Bottom Layer pad to  -0.55 times the smaller of the overall width or height. This will close off the Solder Mask for this pad; 11. Set the Paste Mask Expansion for this Bottom Layer pad to  -0.55 times the smaller of the overall width or height. This will close off the Paste Mask for this pad. That's it done. This is a demonstration footprint: THERMAL\_PAD\_TOP\_COPPER ONLY\_EXPOSED\_DEMO [https://easyeda.com/editor#id=!e48971ab94364709a723a6a1c310cefe](https://easyeda.com/editor#id=!e48971ab94364709a723a6a1c310cefe)<br> <br> The same technique can be used directly in a PCB. Always check the downloaded Gerber zip archive, for example using [https://www.gerber-viewer.com/Viewer](https://www.gerber-viewer.com/Viewer)