I don't quite understand which pads you want to cover with solder mask. Is this for something like a capacitive sensor plate or touch pad? Are they surface mount or do they need a through hole? Are you trying to produce tented vias? Can you make a copy of the footprint public and mark up which pads you want to keep covered with solder mask? One way to do this: Can you make the footprint so that the pads that you want to keep covered are in fact not pads but are sections of track or areas of copper flood of the shape and position you need? You can still connect to the "pads" by giving them the same name as the net you want to connect to. That way they will be treated as traces and covered in solder mask.

This from the EasyEDA Tutorial, might help too: <https://easyeda.com/Doc/Tutorial/ThelatestupgradeofEasyEDA.html#h.ubs94xpocqt1>

They are through hole components, and pads is set to ALL (four) layers. All inner connections are connected with them and my problem is this: I wanna hide pads copper area in top copper layer with solder mask, only the holes in pads are exposed in top copper layer. Pads are with PTH hole (Plating Through Hole) with copper. Greetings: Jarno Piironen

Hmmmm. In theory you could try drawing - in the 'top solder layer' - a patch of solder mask with a hole in it of the same diameter as the through hole and placing it over the pads that you want to cover. I don't know if you could do this as part of the footprint or if you will have to add it manually to each pin you want to hide. The problems - as I am sure you have already found - are that: i) if you edit an existing footprint from EasyEDA Libs > General Packages > Through Hole, although the 'top solder layer' is shown, you cannot edit it; ii) if you create a new footprint from scratch then you do not have the 'top solder layer' is shown at all. **Here's a way to work around these restrictions.** Do: >**New > PCB Lib** Then: >**Document > EasyEDA Source** And you will find you have a JSON text file like this: ~~~~ {"head":"4~1.9.1~400~300~package``pre`U?`Contributor`andyfierman","canvas":"CA~2400~2400~#000000~yes~#FFFFFF~10~1200~1200~line~1~mil~1~45~visible~0.5","shape":[],"systemColor":"#000000~#FFFFFF~#FFFFFF~#000000~#FFFFFF","layers":["1~TopLayer~#FF0000~true~true~true","2~BottomLayer~#0000FF~true~false~true","3~TopSilkLayer~#FFFF00~true~false~true","4~BottomSilkLayer~#808000~true~false~true","5~TopPasterLayer~#808080~false~false~false","6~BottomPasterLayer~#800000~false~false~false","7~TopSolderLayer~#800080~false~false~false","8~BottomSolderLayer~#AA00FF~false~false~false","9~Ratlines~#6464FF~false~false~true","10~BoardOutline~#FF00FF~true~false~true","11~Multi-Layer~#C0C0C0~true~false~true","12~Document~#FFFFFF~true~false~true","21~Inner1~#800000~false~false~false","22~Inner2~#008000~false~false~false","23~Inner3~#00FF00~false~false~false","24~Inner4~#000080~false~false~false"],"BBox":{"x":0,"y":0,"width":0,"height":0}} ~~~~ Find the section: >`"7~TopSolderLayer~#800080~false~false~false"` edit it (directly in the text box) to: >`"7~TopSolderLayer~#800080~true~true~true"` Click **Apply** Then **CTRL-S** to save the empty footprint in **My Parts**. Now you will see that you have an entry in the **Layers** pallette for >`TopSolderLayer` If you make this the active and visible layer you will then be able to draw **Track** and **Solid Regions** shapes (but not circles and, I think, not arcs) on it. With that you should be able to make up a suitable shape to patch over the pads. Making the hole may be tricky because **Bring to front** and **Send to Back** are not available in this canvas. However, even after all that, I am not sure if the PCB manufacturer would allow what you are trying to do to go onto a board: you may need to email EasyEDA support directly to check. Obviously, you would also have to download and look at the Gerbers to be sure if it has worked. Let us know how you get on! :) p.s. It might be worth posting a Feature Request for this.