You will help yourself a lot if you reannotate your components. At the moment they are not consecutive and not consistently prefixed. For instance, you have a load of LEDs that are just numbers with no LED prefix. The led numbers then seem to skip over at least 351 or LED 351: I don't know where the numbering restarts. You also have a bunch of what appear to be resistors but with a T prefix. The text numbering that is scattered about is confusing. For example, why has 330R resistor T9 got R117 written over it in text? This is going to make it a nightmare finding footprints even with the help of the SHIFT+X Cross Probe function. It will help you to read: [https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d](https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d)

i individually numbered as i was having problems figuring out exactly how many components i had vs how many i needed. do i need to go through and annotate all the components respectively to give you a better idea?

i have fixed the identification of leds and resistors. you should be able to see the updated sheet by clicking on that same link. now whats throwing me off is when i go to convert to pcb all the old identifying tags are still there but the sheet (schematic) shows the updated and saved version.

That's because you have simply rewritten all the blue text. You have not reannotated your schematic. The blue text is text. It has absolutely nothing to do with the symbols in the schematic. Delete it. It is the component **Prefix** that needs to be displayed (right hand panel).  and then you must reannotate the whole schematic:  Please read: [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) and the linked documents in it.

i have fixed and saved all the prefix's to the file. i updated to pcb and the leds are going in a ziz zag pattern i saved the pcb layout as far as what im shooting for. 2 rows horizontally 1-351 and the second 352-702. whats the trick im missing? thanks for the help

Please reread: [https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d](https://easyeda.com/forum/topic/Component-autoplacement-into-PCB-3f0f310db0d74a9bbf848953c4c8048d) Convert your schematic to PCB and you get:  Save the PCB. Go back to your schematic and do CTRL+A to select everything in it. After several seconds, everything will light up red. Then do SHIFT+CTRL+X to Cross Probe and Place and after several seconds you will get:  Don't try to move the new arrangement: it will take too long. Instead, just click on the canvas to place the new arrangement when you will get:  Save the PCB and then redraw the board outline. It is not to any sort of physical scale but at least all your hundreds of footprints will be in the order that they are drawn in the schematic which will make it much easier to locate and move to the final placement.

so now that i have this accomplished you can see my board size on the saved pcb layout whats the best way to evenly distribute into the space ive alotted? ive tried the distribute array function but it makes everything go into that zig zag pattern all over again.

"...locate and move to the final placement." If you cannot get them into an array to need using Distribute Array then you will have to move them by hand. Why not make a simpler, smaller version of the project to learn how to use the tools then apply what you have learned to the final mich bigger project? BTW: Your PCB is about 1410mm long and but only about 13mm wide. You should be aware that JLCPCB probably cannot make your PCB:  I am not sure you will find any PCB house that can make a PCB to those dimensions. You will probably have to split the board into lots of smaller ones.

if i copy and paste a group of 24 leds and 6 resistors how do i get them to sync on the schematic? for example the first group will be 1-24 copy and paste and place directly next to 24 and it starts at 48 and decreases down to 25. ive been going to each individual name and rewriting it so it will flow from 1 to whatever number i end up with

Don't copy and paste. Create a Schematic Module and matching PCB Module. Don't try to include net names in either module but do ensure that the Symbol and the Footprint prefixes are identical. Open a new project. Open a new Schematic and save it to the new project. Place the Schematic Modules into the Schematic following the pre-Prefix prompts. Add netlabels where required to uniquely identify nets within and to join nets between module instances. Save the schematic. Open a new pcb and save it to the new project. Place the PCB Modules into the PCB following and adding the same pre-Prefixes that were added to the Schematic Modules. Save the PCB. Do **Design - Import Changes... **and tick the **Also update track's net...** option in the bottom left of the Confirming Importing Changes information window that opens. Click **Apply Changes**. Save the PCB. Route any tracks required to join module instances on the PCB. Save the PCB.