Unfortunately there is no way to do this directly in EasyEDA but your idea of importing the PCB as an image is workable. I can think of two ways to approach this. There's a simple way to do it which gets a design faster but with little support for checking the validity of the final layout. Then there's a longer but much safer way to do it be starting with entering a proper schematic into EasyEDA and then using that to pass the correct PCB footprints and connectivity in the PCB Editor and then using the imported image as a map for where to place the footprints. #### The simple way: You can assign the layer you want the image to be placed on so, for example, you can assign it to the bottom layer for a single layer PCB for through hole components. Then you place component holes where ever you need (where they appear in the original image I suppose). Uou can select component footprints as well as just isolated holes so you can place parts with outlines and the correct hole spacings. You can also place surface mount parts and the pads will be superimposed on the copper from the image. Be aware that any holes or pads surrounded by large areas of copper placed as part of the original image will be hard to solder to because thre will be no heat shunts or `Spokes` automatically generated by pads placed in the copper area as they would be in the normal way of creating a PCB. As you have already realised you will have to be very careful not to accidentally move the image as you place the other parts of the PCB. It may be a good idea to keep the PCB image on a different layer until you are finished and only swap it onto the required layer as the last step to reduce the risk of selecting it and dragging it. Maybe even copy it onto two layers and exactly align them so that if you move one, you have the other as a reference to drag it back to. The Design button (Design Manager) in the left hand panel will be of very limited use because the image cannot be broken into individual nets and renamed as they would be in a normal PCB. If you assign net names to the holes you add so that all the holes and pads that should be on the same net all have the same uniques net name and all those on a different net all have their own unique net names, then you can use the `Connect Pad to Pad` tool and then draw in thin tracks that overlay the tacking in the image to join them up. That way the Design Manager will give information and that will be of more use in helping you verify the integrity of your layout. #### A longer but much more reliable way: In fact if you start off by creating the *schematic* in EasyEDA and do all the work to correctly assign netnames, packages (PCB footprints), Bill of Materials (BoM) information and then pass *that* through to PCB you will automatically get all the pads, part outlines, and holes etc. passed straight into the PCB Editor with all the relevent connections already made. Then all you have to do is to import the PCB image as you have already done, assign it to a layer and then drag all the relevant parts to the right places on the image. As a final step just draw in the thin tracks to join up the pads, overlaying the copper in the image and so remove the ratlines. Then you can use the Design Manager right the way though the process from Schematic to PCB layout and be pretty sure that you have a working, correct layout. The only thing the Design Manager will not show you is of you draw a track that shorts on area of copper in the image to another because the Design Manager cannot be made `aware` of the image so just watch out for that when you draw in the thin tracks to join the pads.

Failed to reply, sorry, but thanks for the advice.