Please see: **Schematic symbols: prefixes and pin numbers** in the EasyEDA Simulation eBook linked to in section (3) of: https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f This explains the significance of the schematic symbol, PCB and spice pin numbering/mapping. If you are making your own schematic symbol, please ensure that it has a completed `Description` field which includes a link to the manufacturer's product page: https://www.njr.com/semicon/products/NJM4558.html and another link to the manufacturer's datasheet: https://www.njr.com/semicon/PDF/NJM4558_NJM4559_E.pdf * Please also note that the JRC4558 is not a part that actually exists, it is an NJM4558 made by JRC New Japan Radio Co, Ltd. For more on this see: https://en.wikipedia.org/wiki/LM386 UTC also make an MC4558: http://www.unisonic.com.tw/datasheet/MC4558.pdf A spice symbol exists for this part in EasyEDA: `MC4558CD_EE` :)

@andyfierman thanks for the reply. I'll dig through that. I did notice the MC4558CD_EE is shown as a square 8 pin symbol and schematic uses two triangles (one with the two extra power supply pins, maybe that's where the confusion is being introduced) which flows better based on where each opamp is in the flow of the circuit. I've assigned the DIP-8 package I'm using, but the symbol doesn't do well with my schematic. I'll review the docs you linked and see if I can sort this out.

For reference in case anyone else has this issue, I think this is sorted out now, and here's what caused the light bulb to flash: In this document: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub In the section labeled: "## PCB and Spice pin numbers" In the quad opamp example shown, I noticed that each opamp had V+ and V- defined, even though there is only one V+ and one V- supply pin in the device. The following sentence elaborates: "Of course there is only one physical instance of each supply pin on the schematic symbol for the quad opamp in this example but each spice subcircuit must have the supply pins explicitly defined." In my dual opamp, I did NOT have V- (pin 4) and V+ (pin 8) defined in my pin map. To correct this I copied the first opamp schematic symbol (with pins 4 and 8 defined), and edited it to define pins 5, 6, and 7, deleted teh U1.2 symbol, and dragged the newly edited symbol in place. With this change the pins on the PCB appear to map correctly. Indeed I need to study using simulation. Not sure if it will work for this circuit or not, but I will explore that.

It is worth noting a trick that one of our users pointed out a couple of years ago. You can place multi-part devices into a schematic just using single part symbols. Suppose you have a symbol for a TL081 single opamp but you actually want to represent the two parts of a TL082 dual opamp. All you have to do is to place a symbol for a TL081, set the prefix (reference designator) to **Un.1** (where `n` is the prefix for that part in your schematic) and edit the pin numbers to be for the first device in the package including the power supply pins. Then place a second symbol for a TL081 (or copy and paste the first one), set the prefix (reference designator) to **Un.2** and edit the pin numbers to be for the second device in the package *including the power supply pins again.* If the symbol has a simulation model attached then they will both have the same spice pin numbering. :)