Remember that nets are joined by net names so check that you have applied the original net names to both ends of any nets that you have now split across separate sheets. This is true of both the normal and the simulation schematics so please see: **\#\#\# Components are connected by netnames** in: [https://docs\.google\.com/document/u/1/d/1OWZVVFRAe\_2NW3WratpkA\_SGuHa5AcRow5ZRfvcoVTU/pub\#h\.2jxsxqh](https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub#h.2jxsxqh) This may also be part of the problem: [https://easyeda.com/forum/topic/Error-in-Update-PCB-with-subparts-across-more-than-one-schematic-sheet-fbfcece4060148cd8d9bc3a2228bbc68](https://easyeda.com/forum/topic/Error-in-Update-PCB-with-subparts-across-more-than-one-schematic-sheet-fbfcece4060148cd8d9bc3a2228bbc68) If this does not help, I suspect that you will have to submit more information in a Bug Report for this.

It is probably caused by my way of dividing a large scheme into smaller ones. I did it so (because I can't imagine doing it any other way) that I cloned the scheme. As a result, I had duplicate diagrams with the same element names, etc ... which of course information about the duplicates. Next, from diagram A I deleted the one which is not necessary for B and vice versa. As a result, the chams are ok and together they give what I need, but probably some element identifiers (invisible for the user) caused the program to recognize them as new (despite the fact that the names have the same) and placed on the PCB outside the board.

@Hypno, I did a little experiment with a schematic with one pair of resistors cross connected to a second pair of resistors. I created a PCB for it and then cloned the project and split the schematic across 2 sheets and then updated the PCB in the cloned project with no problems: EasyEDA said that the PCB and schematics were the same and there were no DRC errors. I think the way to do it is to clone the whole project then split the schematic in the cloned project into smaller sheets _making sure that you cut and paste rather than copy schematic segments so that you do not added new parts with new prefixes._ Also as I said above, _you must also ensure that your split nets are properly labelled at both ends so that they join up across the sheets after being split._ When you split a net, even if one part of it has a netlabel on it, it does not inherit that netname. When you cut or copy and paste it into a different part of a sheet or a new sheet, then any unlabelled nets will be automatically renamed to a different unique netname and so in effect will create orphaned connectionsa dn will generate DRC errors when checking the Design Manager.

@Hypno, Strongly recommend that you update your version of Firefox. It is now at V70! :)

@andyfierman You don't have to worry ;-) I have this version of FireFox at work for other reasons. I design at home in Chrome.

I just think the words "cut and paste" are the key. Suppose I have ABC elements on the schematic. With my approach, I have three schemes with ABC content for a moment, i.e. clearly duplicates. Then I remove what is unnecessary from individual schemes and as a result I have the first scheme with the contents of A, the second with B and the third with C. In your approach, you have a scheme with ABC, you add another but empty and by Ctrl + X and Ctrl + V you move from one to the other. In this way, you NEVER even have duplicates for a moment. And the system somehow has to deal with these duplicates, that is, change the names. However, my initial scheme was such that my approach was definitely easier (I did not have functional blocks in the form of square regions). Now I have explained myself the problem :-)

Yes: EasyEDA automatically renumbers newly placed or copied and pasted parts to avoid duplicate prefixes. There's a little info box slides up in the lower right of the Editor window to warn of this but it is easy to miss it. Automatically changing duplicate prefixes are mostly a good idea but maybe less so for other situations. If you clone a schematic sheet into a project which contains duplicate prefixes then these are not automatically renumbered but they are flagged up as duplicate prefixes when an attempt is made to convert to or update a PCB. Anyhow, it's good that you're sorted now. :)