In your schematic, R1 is not connected to R3. The bottom throw of the lower 3 pole switch bank is shorted to ground. Is that intentional? Why do you have red join dots on every component pin? If you snap the end of a wire directly on the active pin end then you will not get these superfluous and distracting join dots. Why do you have a second schematic with the same component numbers but with some of the wires removed? When you click Convert to PCB, in the Schematic Editor you will get duplicate prefix warnings. This suggests that you have not created the PCB from your schematics or that you have added the second schematic after creating the PCB from the first one. Do not place copies of schematics or extra schematics in the same project because they will all be converted into a single PCB. If you added the second schematic after converting the first to PCB and then were to do Update PCB from the Schematic Editor or Import Changes from the PCB Editor then you would get duplicate prefix and component errors. Please use the schematic and PCB Design buttons to check and compare the connectivity of both the schematic and the PCB. Please also use the Cross Probe tool.

Please check your schematic, the R1 connection is broken 

@andyfierman   Andy, you took a look when I was trying everything. I tried every way to get a switch that works in my schematic. I have a complete drawing of the part with all dimensions. The problem I have now is that the part does not show what pin number is on which pin in the schematic symbol, so it would be a lot of trial and error, but that should not be the case. Doesn't the people who make the software do anything to get some common parts that are correct in the library?  I already ruined that first set of boards because I used a Transformer that had no holes in the definition of the part, it just had dots, so that was easy to fix, but the PCB people didn't point that out o me until I went to submit another PCB with the same transformer missing the holes. So that does not happen again. The switch I am using is from the library, and some how it is way wrong when it goes to  the PCB. I would need to edit the part, but since they left the pin numbers off of the schematic symbol, it is very difficult to know what pins to change.

I fixed the schematic, and the switch still comes up wrong. One simple way to see it is that there is one short between one of the wiper pins and a pin direct across from it. It in no way represents the schematic switch wiring.  [https://easyeda.com/joe.massimino/20db-attenuator](https://easyeda.com/joe.massimino/20db-attenuator)

@andyfierman   I   have a part being edited, what I can't see is how to edit both the schematic part, and the PCB part.  Right now I can see the silkscreen layer as a rectangle around the part. I have edited all the pins, shapes sizes, and spacing. I am getting to the point that I would want to edit the schematic symbol to match with the PCB symbol and add it to my own parts list once it is correct.  If there is a video tutorial on creating parts , along with audio, that could go a long way in people helping themselves.

 @andyfierman  This was all about the switch, and nothing more,  i fixed the schematic, but you looked at it when I was attempting to fix my own problem, which I did not. I deleted all wiring and tried to put the parts on a circuit board and wire it myself, but the system will not let me do that.  I am very close to having my PCB image ready, I'm just not going to know how to link a schematic image to it for my library, and use in my board.

If you ask a question about a project, please don't change the content of that project while people are looking at it to try to help you. If you need to work on it then clone it to another public project and refer to the clone in your posts.

"I have a switch that is a dP3T slide, and the two poles come from a BNC.  When i examine the PCB, i see connections that don't match the schematic they came from.   How can that be?" In your schematic, you have not identified: 1. a manufacturer or supplier  2. a manufacturer or supplier part number for the DP3T switch and for the BNC connector. Therefore you have no manufacturer or supplier datasheets to refer to from which to specify the pin numbering of these two components. This is particularly important for the DP3T switch. You do not even know of the DP3T switch footprint actually matches any available physical component. Therefore you have no idea how to map the pin numbering of the schematic symbol to the locations of the corresponding pins in the PCB footprint. I have already explained in: [https://easyeda.com/forum/topic/Part-used-is-not-found-so-I-want-to-edit-a-part-so-it-can-be-mine-how-do-I-do-that-80f71b52df2e4cb89affd38a765ba78d](https://easyeda.com/forum/topic/Part-used-is-not-found-so-I-want-to-edit-a-part-so-it-can-be-mine-how-do-I-do-that-80f71b52df2e4cb89affd38a765ba78d) that the first step in choosing parts has to be to identify the real physical part that you want to use on the PCB. You have not done that for your switch so you are not in a position to ask questions about it. That's like me saying that I'm going to build a car and then asking what the tyre pressures should be when I haven't even specified which wheels I'm going to use.

I do have a detailed engineering drawing the the switch. I created a PCB  foot print that will fit the switch.  What I don't have is the schematic part that allows me to wire it into ky circuit, and turn it into a circuit board the way it should be.  The BNC, is two pins, and Know how it goes, so it is wired correctly. What I ask you now, is if I go to Mouser, or Digikey, and get a switch from a big company like switchcraft, or one of the others, is there and easy way to get that part into my schematic, or  do I have to build an image for it? What I tried to do today, was click on the switch in my schematic and edit it, only after I did the complete edit to make it correct, it would not retain what I did.  So why was the edit there if it does not retain anything? So process should I follow to get a switch that will plug into the software and let me use it?

1\. First get the datasheet for the part you're going to use\. 2\. If you can find a PCB footprint the the EasyEDA library that is the right size then open it in the PCB Lib Editor and then edit the pin numbering to match that of the part in the datasheet and save it with the part number you're using\. 3\. If you can't find one the right size in the library then you can either edit one that's close to it or create a new footprint from scratch in the PCB Lib Editor and then save it with the part number you're using\. 4\. Then you can either select the schematic symbol in your schematic and click on the package attribute and when the footprint pinout manager window opens\, enter the name of your footprint in the search box in the right hand side and when it is found\, click on it to tell the manager that that is the footprint you want and then edit the schematic symbol pin numbers so that they match those of the PCB footprint\. Click Update and then close and that should have associated your switch symbol in the schematic with the PCB footprint and set the correct pin mappings\. Save your edited schematic symbol with the exact same name as that of your PCB footprint\. 5. **Or** find the switch schematic symbol in the library and open it for editing in the Schematic Lib Editor. Then edit the pin numbers to match the pin mappings of the datasheet and make the pin numbers visible on the symbol. You can make the pin names the same as the numbers or anything you like or just even leave them blank. You can make the Spice pin number alone or delete them as there is very rarely a need to for a model of a simple switch. Next, click on the package attribute and when the footprint pinout manager window opens, enter the name of your footprint in the search box in the right hand side and when it is found, click on it to tell the manager that that is the footprint you want and then click Update and then close and that should have associated your switch symbol in the schematic with the PCB footprint and set the correct pin mappings. Save your edited schematic symbol with the exact same name as that of your PCB footprint. 6\. Delete the symbol in the schematic and replace it with the new one\. 7\. Do Update PCB\.

I'm going to print your instructions and see how far I get.  My main issue is the auto routing on the part I have, it does not match the part, so it wires everything wrong when it comes to the switch. I can't believe that my entire project is being held up by a simple switch.