Apart from the passive and maybe the 1N4007 diodes, none of the symbols will have spice models associated with them because they are not from the Spice Symbol library. You have used non-standard schematic symbols for the slider pots which makes the schematic a little harder to read but other than that, you have got power supply decoupling in place and the schematic is nicely laid out which will make it easier to follow the connectivity. Your next step, while waiting for other comments and before even thinking about doing **Convert to PCB** is to go through the checklist (4) 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)

Other then the slider pots all symbols are from the easyeda library, infact, most of them are in the eelib.

To clarify: Except for resistors (excluding variable resistors and pots), capacitors and inductors, symbols used in schematics will only have spice models associated with them if they are selected from: 1. The Spice Symbol library; 2. The EELib **but only when selecting parts in Sim mode. **

Curious: why did you not use the pot symbol from the EElib and just edit the name and Footprint?

Some more observations. 1) All your opamp inverting and non-inverting inputs are reversed. 2) If your slider pots and the master left/right pots are not on your PCB then they should not be in the schematic. If a component is on - or forms an integral part of - the PCB then it must be represented in the schematic. Conversely if it is not on - or does not form an integral part of - the PCB then it should not be in the schematic from which you intend to convert to a PCB. Please see (2.3) 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) 3) You have tried to create a simulation schematic by setting the schematic editor to Sim mode but, as already pointed out, you have not used Spice Symbols, you have used a selection of Schematic Symbols and EELib symbols. If you want to simulate a circuit then you must read (3) 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) 4) By creating the schematic in Sim mode you have no package or other BoM information available and you cannot convert your schematic to a PCB. To convert your schematic to a PCB you will have to save it, close it then reopen it in Std mode. Then you will be able to see and if required, edit the PCB Footprint and BoM information for each Schematic Symbol. Then, once you have gone through the checklist in (4) 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) You will be in a position to do Convert to PCB. Then as you work on the PCB and as you complete it, go through the checklist in (6) 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) Then you can run the Gerbers, check them using gerbv and complete the checklist (6) above. Then check everything again. Then submit the board for manufacture after reading the instructions at the bottom left of the JLCPCB submission page.

FYI, there does not appear to be an unencrypted spice model available for the LME49720 (i.e. one that will run in anything other than Pspice or possibly TINA). You can use the EasyEDA opamp5pee parameterised model and adjust the available parameters from the datasheet values for the LME49720. This will allow you to simulate the basic design andverify the connectivity of the schematic but you will not be able to accurately model noise and distortion performance using that model.

Over the past few days I have been trying to find spice models for a few dozen other IC's and found that NONE were available in the spice directory other then a few user contributed one's. Wouldn't it make more sense that if LCSC sells the components that easyeda should have a proper spice model for them. Maybe it's just me being silly but it would make sense.

"Wouldn't it make more sense that if LCSC sells the components that easyeda should have a proper spice model for them." It might make sense but EasyEDA does not have the resource to do that at the moment. The [Simulation Tutorial](https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub) does however describe how, if there is an unencypted model available for a device, you can associate a model with an existing Spice symbol.