@ainfirdaus, Welcome to EasyEDA. For small, hand soldered projects it is nice to have the value of the component printed on the PCB but there is not always enough space to do that. Standard practice on professional PCBs is to show some or part of a package outline and a reference designator or prefix such as R23, C3, Q7, U12. Like this: https://easyeda.com/editor#id=a0cf7282b35140928ab93bc65c4b9cfb or: https://easyeda.com/editor#id=787e693bbdad44dd8057f04e2dd8e585 In fact on some high density PCBs and on many commercial PCBs even the prefixes are omitted. The correct way to deal with hand fitting of parts onto a PCB is to use the Bill of Materials (BoM) as your component prefix to part name or value cross-reference, not the schematic. The BoM specifies what physical parts you buy for each instance of each part and therefore exactly which part is fitted into the PCB location specified by each prefix. If you follow the checklists given in: https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f your schematic will generate a BoM that accurately maps the correct value onto each instance of each part and the package associated with it and therefore exactly which physical part is to be fitted (or not according to the `Mounted` attribute in the schematic) at each location on the PCB. If you really need the part value printed on the PCB there are several ways that you can do this. 1. You can manually enter the value text directly onto the PCB silkscreen. This will appear on your onscreen and printed (onto paper) PCB view. It will also appear on the physical PCB. 2. You can manually enter the value text onto the `Document` layer of the PCB. This will appear on your onscreen and printed (onto paper) PCB view but will not be printed onto the physical PCB. 3. You can create dedicated PCB packages for each unique valued part and include some text in the package drawing (PCB Lib) that shows the value and then assign those to the relevant schematic symbols. 1. For example you have 4 resistors and three values: R1=1k, R2=10k, R3=3.3k, R4=1k. 2. You create 3 packages named `Res_1k`, `Res_10k` and `Res_3k3`. 3. Each package includes the value as text: `1k`, `3.3k` (or `3k3`) and `10k`. 3. You assign `Res_1k` as the package used by the symbols for R1 and R4 in the schematic. 4. You assign `Res_10k` as the package used by the symbol for R2 in the schematic. 5. You assign `Res_3k3` as the package used by the symbol for R3 in the schematic. 3. Then when you create the PCB, the packages appear with the correct prefixes but also with the correct values for each part in the PCB. This is however a very labour intensive task.

It is also good practice to 'kit' the PCB parts before starting assembly. In my example above, this simply means that you group together 1k resistors - maybe in a little bag or tray - and label them `R1, R4` and then label the 10k as `R2` and the 3.3k as `R3`. This is a trivial example but on more complex boards this saves a huge amount of time during assembly.

Hi We will try to solve this in the future. at now, you need to add a text for each component at PCB. thank you .

I am just starting out with easyeda, and this was something I wanted to do. Some of the best boards to assemble are those that have component values silkscreened. This is also very useful when you burn a component and need to replace it. A simple menu option to allow prefix and/or name would be really nice.

And it looks like it has been implemented. Nice.

I just create my own parts with a designator where I want it - for instance see part AXIAL\-0\.4\_MDB\_300K