The problem is with the 'power pins' on the symbols for opa2277PA.2. The quick workaround is to not connect anything to the two power pins on the U1.2 and U2.2 symbols. * opa2277PA.1 correctly includes power pins. * opa2277PA.2 shows two pins in the same places as the power pins on opa2277PA.1 but which have no numbers and that are not listed in the 'i' Edit Symbol tool:  opa2277PA.2 should either: 1) include power pins exactly as shown on opa2277PA.1 or; 2) should not show power pins at all. As opa2277PA.2 is drawn at the moment, users connect power to the un-numbered and unlisted power pins on the symbol with then creates a 'This netlabel is not connected to any pin' warning in the schematic Design Manager for the positive and negative supply pins that is very hard for them to trace and understand. * The correct solution is for LCSC to fix the symbol as described below using the Report Error tool but that is limited to only 256 characters and it is hard to report the error clearly in so few characters. Therefore I have submitted a Bug Report for this symbol (which may apply to others). [https://easyeda.com/forum/topic/Power-pins-on-opa2277PA-2-two-symbol-for-C47994-opa2277PA-2-are-wrong-bfed244ca2be461abcfbdb4b79dcf0ef](https://easyeda.com/forum/topic/Power-pins-on-opa2277PA-2-two-symbol-for-C47994-opa2277PA-2-are-wrong-bfed244ca2be461abcfbdb4b79dcf0ef)

BTW: what purpose do the back to back 1N4148 diodes across the input and output serve? They have a reverse breakdown of somewhere north of 75V so they are not going to protect anything in that configuration. Did you intend to fit zener diodes instead?

As to how to simulate your circuit, it is eminently possible but you need to read and play with the examples in the Simulation Tutorial, (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)<br> <br> before attempting to. :)

@andyfierman thanks man! It was driving me crazy!! Maybe i could replace those ICs with any DIP-8 with the same pin orders and a correct drawing just to have a working schematics (so i can order this PCB) and then soldering the OPA2277 (which Is also an equivalent for the original TL1112 that i cannot find anywhere)? For the diodes i was copying the schematics i found but now i understand that they are useless. Should i insert two zener (IN and OUT) or i can simply remove them?

Hi we removed these two lines at the subpart symbol, that make the pin chaos

@difesa98, Two solutions: Use the corrected power pin OPA2277PA schematic symbols that I have just created (and omit the U1.2 and U2.2 supply connections):  or use these LMC6482 Spice Symbols which will then help you to simulate the design:  Creating a schematic that can be simulated and can also be converted into a PCB with full BOM output support or converting a non-simulation schematic (created in STD mode) into a simulation schematic (in SIM mode) is quite tricky because it will have to include something to represent the pots and switches etc., which have all the right BOM and Footprint information in STD Mode but is supplied by symbols which are not simulatable in SIM Mode. If the parts of the non-simulation schematic which need to be simulated can be broken up into separate sections connected by netlabels, each of which can be turned into single sheet that can be simulated on it's own as described below, then that can be helpful otherwise everything that needs to be simulated has to be drawn together in a single sheet. It is also necessary to add power supplies, signal sources and off-PCB loads into the non-simulation schematic in such a way that they are excluded from the BOM and are either not converted to footprints in the PCB or are assigned footprints that represent the means by which they are connected into the real PCB such as battery holders and signal jack sockets. This latter option is neat but can get messy if they are connected by individual solder pads on the board rather than using a single footprint that represents all the necessary pads for those connections or if there are more pads on the footprint than there are pins available on the Spice Symbols (the green 'X', Not Connected, symbol cannot be used in spice simulations: it causes errors). Except as just described above it is also necessary to use a separate schematic sheet to exclude the stuff like connectors which do not need to be included in the simulation schematic in SIM Mode. It is recommended to use the basic voltage sources and voltage probes from the EELib or the Spice Symbol Library instead of the EELib power supply and oscilloscope widgets. To achieve this, it is **essential **to read - and play with the examples in - the Simulation Tutorial (3) and also (2.2) and 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) in order to understand how to: * create successful simulations in EasyEDA and; * use the **Convert to PCB** and **Add into BOM** attributes. **Here's a way to create a simulatable schematic which can also generate a correct BOM and which can be seamlessly converted to a PCB is to:** 1. Create a complete single sheet non-simulation schematic, with netlabels, in STD mode using symbols from any of the Symbol libraries. That way you get proper BOM info in your schematic. However, the diodes, transistors, amplifiers, pots and switches will not be simulatable yet. 2. Make a list of the Supplier and Manufacturer, Supplier and Manufacturer part numbers and Footprint attributes of the diodes, transistors, amplifiers, pots and switches. 3. Add a second sheet then cut and paste all the connectors, mounting holes, through hole pads for external wiring etc. from the first sheet, onto the second sheet just connected to the first sheet using netlabels. 4. Make sure that the relevant netlabels exist in both sheets. 5. Save it. 6. Swap to SIM mode and replace the the diode, transistor, amplifier, pot and switch symbols with equivalent simulatable parts from the Spice Symbol Library.  7. Add the necessary signal sources and voltage probes from the EELib or Spice Symbol Library and the spice directives. 8. Save it. 9. Swap back to STD mode and then edit the Supplier and Manufacturer, Supplier and Manufacturer part numbers and Footprint attributes of the replacement Spice Symbols for the diodes, transistors, amplifiers, pots and switches to those noted above. 10. For all **on-PCB** components that form part of the PCB Assembly, set the **Convert to PCB** and **Add into BOM** attributes to **Yes**; 11. For all **off-PCB** components that form part of the finished assembly, set the **Convert to PCB** attributes to **No** and the **Add into BOM** attributes to **Yes**; 12. For all **simulation only components** such as the signal and power supply sources, set the **Convert to PCB** and **Add into BOM** attributes for to **No**; 13. Save it. That completes the creation of a non-simulation schematic with all the required BOM and Footprint information which will correctly generate a BOM and which will convert seamlessly into a PCB in STD mode and contain all the Spice Symbols so that when you run it in SIM mode it will be simulatable. Before doing **Convert to PCB...** follow the Essential Checks (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) Before submitting the PCB for fabrication and/or Assembly, follow the Essential Checks (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)

@UserSupport, Thanks!