**Print** and **Export > PDF...** from the online version, both work fine for me using Chrome, Chromium and Firefox.

I am using Chrome, and not only does printing not work, but I put copper areas on the board, and the outline is there, but it does not fill. I will save all my work, then reboot and open it again.

@andyfierman I ran an update on my Windows 10, then checked for another after reboot, then opened my EasyEda project and I not only don't have my copper areas filling in, many of the traces are not there, but I know they are as I tried to move something on the board, and it said I was on top of a trace that I can't see. I know you say your EasyEda is working perfectly, but have you tried to create a new schematic, and do some of what I said does not work?

@andyfierman Not only that, after careful inspection the few traces I can see are wrong, for instance, i now have a trace between 13vdc, and ground, how did that happen? It is not that way on the schematic and I went to the schematic and told it to update the PCB, and it did nothing.


Notice the only traces being seen, and the one where 13vdc is attached to Ground.  I removed the trace and ran autorouter again, and it did the same trace over again.  Andy, you might work for EasyEda, and not wanting to admit that some servers might be corrupt, I doubt we are on the same server.

@joe.massimino, I primarily provide simulation models and support for EasyEDA. I help out on the forums in my spare time. I have no knowledge of or access to any of the cloud server systems or admin. 1. Please make public copy of a project that demonstrates this issue available or; 2. Add support as a team member or; 3. Add me as a team member or; 4. Email a downloaded zip copy of your project to either support or me.

I don't see a place to add a team member. I looked through all menus.

[https://easyeda.com/joe.massimino/antennaswitch](https://easyeda.com/joe.massimino/antennaswitch)

[https://easyeda.com/joe.massimino/antennaswitch](https://easyeda.com/joe.massimino/antennaswitch)

[https://easyeda\.com/editor\#id=\|649f60d467494cae872c81f9b89d908f\|15554a162b934a7381e75565b6453e24](https://easyeda.com/editor#id=|649f60d467494cae872c81f9b89d908f|15554a162b934a7381e75565b6453e24)

Sorry, they did not make adding a team member so easy as just knowing who you are. I tried to add the project path, but nothing worked, even though i got the paths from the project.

This is why we have a Tutorial: [https://docs.easyeda.com/en/Introduction/Project-Member/index.html](https://docs.easyeda.com/en/Introduction/Project-Member/index.html) [https://docs.easyeda.com/en/Introduction/Share-to-Public/index.html](https://docs.easyeda.com/en/Introduction/Share-to-Public/index.html) I can however, now see your project and you have successfully added me to the project team: [https://easyeda.com/joe.massimino/antennaswitch](https://easyeda.com/joe.massimino/antennaswitch) I will look at it when I have a few minutes.

@joe.massimino, To ensure that I have reviewed your project at - or as near as possible - to the time when you made it public and not after you may have made any changes to it, I have taken a copy and have reviewed that: [https://easyeda.com/andyfierman/antennaswitch](https://easyeda.com/andyfierman/antennaswitch) The following is my review of your project at that point. It comprises three sections: Schematic, PCB and Conclusions. **Schematic.** Basically the problem is that you have not gone through the checklist (4) of **Essential Checks before doing Convert to PCB…** in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) 1) Your schematic is drawn badly. Every wire overhangs the symbol pin to which it is intended to be attached. This makes it unnecessarily hard to read:  This is expressly identified as bad practice in the checklist (4):  2) Your schematic is incomplete:  3) You have not checked the schematic using the Design Manager. If you had then you would have found the short across C10:  Which is why you have a connection between the 13V supply and ground. 4) You have not applied net labels to any of the nets which is recommended in the checklist (4) to help identify nets in both the schematic and the PCB and to help identify connectivity errors. This has impacts in the PCB that are identified later. 5) You have not checked, as advised in the checklist (4), the Schematic Symbol pin to PCB Footprint pad mappings of the relays and the BC817 transistors using the Footprint Manager and against the datasheets:   [https://assets.nexperia.com/documents/data-sheet/BC817_SER.pdf](https://assets.nexperia.com/documents/data-sheet/BC817_SER.pdf)  Therefore, the connectivity of the PCB is wrong compared to what you intend in the schematic. As an aside, your schematic may be over complicated for what you are trying to achieve. You have two SPDT relays driven in anti-phase by an NPN and a PNP switch so that when relay 1 is on, relay 2 is off and vice versa. You could drive both relays from one NPN switch transistor and just swap the normally open and normally closed relay contacts over on relay 2. That saves the BC807, a 1N4007 and a few other passives at the expense of having a roughly 65mA drain when the relays are on and about 5mA when they’re off as compared to a more or less steady 35mA with either relay 1 on and 2 off or vice versa. Also, I appreciate that you are switching RF signals but do you need to have decoupling caps at the collectors of the relay switching transistors to both 13V and ground? **PCB.** “...opened my EasyEda project and I not only don't have my copper areas filling in, many of the traces are not there, but I know they are as I tried to move something on the board, and it said I was on top of a trace that I can't see. “ This is because you have turned off the visibility of the bottom layer:  7) If your PCB is for RF then you need a good, solid, well connected area of ground plane. Don’t do a munge of bits of track and bits of ground plane. Just put as much ground plane as you can on both sides of the board. 8) Sort out your net labelling in the schematic to avoid this kind of net name/copper area name incompatibility in the PCB:  9) You have several unconnected ground plane areas:  This is why you have copper areas that are not filling. 10) You have not gone through the checklist (6) of **Essential Checks before submitting a PCB for manufacture** in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) If you had you would have found that you have this DRC error:  **Conclusion.** “...I know you say your EasyEda is working perfectly, but have you tried to create a new schematic, and do some of what I said does not work?” Yes and subject to all the above errors and mistakes: yes; EasyEDA does exactly what it is supposed to be doing. In conclusion, the mistakes and errors that I have identified in your project are nothing to do with the operation of EasyEDA and it’s servers. I am sorry to be blunt but they are all due to your failure - for whatever reasons - to learn how to use EasyEDA effectively and to carry out your work  following the numerous Tutorials and other guideline materials: all of which you have been pointed to repeatedly in your other posts over the last year or so of your use of EasyEDA and many of which have included detailed and time consuming responses, as a look back over [your posts](https://easyeda.com/joe.massimino/topics) will confirm.

Did that explain all the missing and mis-directed wiring in the board. that all happened after I saved the board, and updated my computer os, then came back to it. I  will look it over and make corrections.  I don't see why all the connections were not there.

I see where when I click on a wire, and adjoining to it wires don't respond, like they are not connected. Is there a way to edit the wires together, or do I have to delete it and make it all one connection in one swoop of wire?

I don't understand your issue. Please post screenshots or preferably. an animated gif to illustrate it.

Ads for all those problems you identified, they all occurred on their own, after I updated my computer, then checked back in. That is when I got disgusted with the software, and what was going on. I think that they are not working in China, and nobody is keeping watch on the servers.

Please go back through your **Historical Records...** and make an earlier uncorrupted copy of it public so we can compare them. 

Andy, I did figure out what was a wrong with the wiring, and now it is working as it should, except the way I can get copper fill, is if I do the entire board. I actually want to fill parts of the board but not the entire board.  Is there a way to do that?

Draw the copper areas where you want them. Set their net names to the nets they are to connect to. Make sure there is at least one pad, via or track of that net name in each copper area. Set keep island=no. Set spokes not solid. Rebuild all copper areas.