Hi, This is private project, I can't check it, but I know what you want to do. Can you tell me how many copy do you need? You can order 10 pieces PCB from EasyEDA, you just need to pay for $10. Dillon

Hi gordonwolff, Sounds like you're having fun with EasyEDA! It is possible to copy and paste a complete layout but as you have found, the nets in each copy will ratsnest back to the original. This is because they will all have the same net names. To get round this you can edit the net names in the copy to, say, add a suffix of 1, 2, etc,. for each copy. This is very tedious even for a small board so what you can do is a cross-document copy of the whole layout (Ctrl+A then Ctrl+C) and paste it (Ctrl+Shift+V) into a new, separate PCB canvas and then, using a text editor, do a search and replace for the net names in the **Document > EasyEDA Source** file then apply it to the new copy. Then copy do a cross-document copy of the whole layout (Ctrl+A then Ctrl+C) and paste it (Ctrl+Shift+V) back into the original PCB layout and palce it where you want. That way the net names will be unique in each copy. In principle I think that will work to get you a workable layout but you might need to contact `support@easyeda.com` to check that (a) there isn't a better way to do this as I've not tried it all the way through and (b) that there are no other complications in generating the Gerbers caused because the total layout now no longer relates to the original schematic. I recommend you clone the whole project and play with a copy before letting rip on the real thing. Or maybe even just try a very simple test schematic and pcb just with a couple of components on it. Do let us know if you have problems or if it works! :)

Hi gordowolff, Another point about putting multiple copies onto one PCB. Using the technique I described above, you may need to delete the original single board outline and put an overall board outline around the multiple copies. You'll probably also want to then put some silk screen markings to show where to cut the panel up into individual boards. Maybe even put rows of drill holes to assist in breaking them apart (though that puts the cost up a bit). Bearing in mind what Dillon says about how you can order multiple PCBs from EasyEDA, it may just be simpler to do the single board and see how much it costs for 10off or so. Why not do a single PCB and then see what cost estimate EasyEDA gives you when you run the Gerbers and then click on the **Order...** shopping cart? You're in no way committed to buy anything at that point but you will get a cost estimate in the dialogue window that it opens. One more idea: it is possible to create panellised PCBs just from the Gerbers. This saves all the messing about with the net renaming. Since EasyEDA suggests you download a copy of the FOSS gerbv package, this article may be of some help: [Panelize & Merge Gerber Files with Gerbv (Free Software)] You will have to check if EasyEDA can accept Gerbers created that way with `support@easyeda.com` [Panelize & Merge Gerber Files with Gerbv (Free Software)]: http://www.tristantech.net/articles/gerbv/

Is there a better way to do this now? The easy eda source text file for my project is thousands of characters long and has multiple instances where searching the text string name of a component comes up with coincident items that are unrelated so this method isn't workable.

You can save your single small PCB as a module then paste multiple copies onto a new PCB project. You'll have to delete the board outline of the individual module and put an overall outline round the array. See: https://easyeda.com/Doc/Tutorial/PCBOrderFAQ And look for the sections on panelization and V cutting.

@andyfierman Thats exactly what I was looking for. Thanks again mate.