@Alphabetix, A single opamp has a single subcircuit. For a dual opamp you have to create a subcircuit which refers to the single opamp subcircuit and maps the pins onto the dual opamp package. Here's an example: ><https://easyeda.com/normal/How_to_build_a_spice_model_for_a_dual_opamp-8MTNHZTN5.png> in: ><https://easyeda.com/andyfierman/Public_user_help-ZmaYWw5FD> (Sorry it's posted as an example but I couldn't persuade the Comments box to show the whole netlist without it messing up the syntax) Quesions? Just ask. :)

I've actually (almost) solved my problem - I took a guess and it worked. I'm adding 2 TL071 op amps to my schematic, calling them U1.1 and U1.2 and mapping these to one DIP8 pinout. This is working in the emulator and also perfect in the PCB. The only issue I have left is how to make the supply rails for one of them invisible in the schematic. I'm currently connecting the extra pins which doesn't affect the generated PCB but, just for completeness it would be nice not to have the pins duplicated. BTW thanks very much for your help

If you create the TL071 symbols so that their power pin **Electric** attributes are flagged as `Power` in the symbol editor, then when you place and select the device in a schematic and, when you type `i` and the **Modify your symbol information** dialogue box opens, ticking the **Hidden Pin:** box will hide the power supply pins for that symbol. If the power pins are named `V+` and `V-` then as long as the relevant supply rails have netlabels or netflags of *exactly* the same names, the supply will connect to the symbol. If you have devices that have to run from different supplies but who's symbols have the same supply pin names then to avoid the problem of having two different sets of rails that have the same names, you can edit the supply pin names of the relevant symbols in your schematic using the **Modify your symbol information** dialogue box. So, for example if you have two TL071s (U1.1 and U1.2) that have to run from +/-15V and another (U2) that has to run from +9V and ground. By labeling the +15V rail to `V+` and the -15V rail to `V-`, labeling the +9V rail to `+9V` and then renaming the positive and negative power pins of U2 to `+9V` and `GND` or `0` respectively then the supplies are given unique names and connect to the correct pins on the respective devices. Do you follow?

>I took a guess and it worked. I'm adding 2 TL071 op amps to my schematic, calling them U1.1 and U1.2 and mapping these to one DIP8 pinout. This is working in the emulator and also perfect in the PCB. You are genius, this is a good idea. BTW, you can try to order PCB from EasyEDA. Look forward to server you. https://easyeda.com/forum/topic/Whos_ordered_PCBs-L71VduMGY

Andy, that's the last piece of the puzzle. It worked exactly as you described. Thank you so much for your help. Dillon, when I have the project working as I want I will certainly be using your PCB services.

@Alphabetix, Your inspiration of using the Un.m idea for schematic symbols in spice simulations actually solved this same problem that I had during the Tesseract amplifier project development. I had not thought to try the same approach that works in simple schematic symbols with symbols that have spice models associated with them (the spice symbol creation menu does not offer that option as it does in the normal schematic symbol creation menu). Once I realised that worked I then tried the pin hiding features to check that they worked in this application and it was while I was doing that, it finally dawned on me exactly how to connect hidden pins when there are multiple supplies for different devices with the same part type. So your question and answering it has been a big help to both of us! If you need any further help, just ask. :)