Please re-read the preliminary remarks in the Simulation Tutorial. The opamp symbol you are using almost certainly has no model associated with it. There is however an LF356EE model in the spice symbol library.

@andyfierman Andy, As I said I got that op amp out of the library/SCH libs/system  , which I read somewhere most should have ngspice models associated. So while looking through the library, is there a way to tell if a symbol has a ngspice model attached?  {This has proabably been asked and answered now many times} THANKS for the help!

@phillman5, Most simulatable symbols can be found by searching for the tag: SpiceSymbol But some of the very symbols created very early in the life of EasyEDA do not have tags. Spice symbols have a small blue "s" inside them in the left hand side of the Search Libraries results list but many these are user contributed and are wrongly constructed so simply do not simulate. The Spice Tutorial is very specific about where the simulateble Spice symbols can be found: "Schematic symbols with spice simulation models attached to them can now be found using the: **Libraries** button in the left-hand panel or; **SHIFT+F** in any editor window. then click on `SCH Libs`, hover the mouse over the `System` class then slide down and click on any of the grey buttons under the **Spice Simulation** heading" If it is not from one of the buttons under the **Spice Simulation** heading, then it is not a simulatable symbol.

@andyfierman Andy, I have followed the spice tutorial and your directions above,  library/SCJ Libs/   hover over System   go down to Spice Simulation.  There I find  5 gray boxes: Spice Gate   spice Source   Spice Discrete   Spice Regulator   Spice Miscellaneous Though I don't expect to find the op amp LF356N (or as you stated above an LF356EE that is available) in most of these, I have looked in all of them, and I don't find the LF356EE you mentioned was available in the spice symbol library. According to the tutorial I did look at the available spice models [https://docs.google.com/spreadsheets/d/1KM28xzXwgQeUUj3zRMlth9BN-vs6Q98KBk1FHXmf58U/pubhtml](https://docs.google.com/spreadsheets/d/1KM28xzXwgQeUUj3zRMlth9BN-vs6Q98KBk1FHXmf58U/pubhtml) and did see it there. Does that mean I need to associate the model with a spice symbol according to the tutorial directions?  Where do I find the .model Also I have found several references to a 'super menu' but I don't see that on the UI.  Searches show some images of screen shots show it on the far right, other far left.  I simply don't see it anywhere.

If you place a 5 pin opamp from the spice miscellaneous library (but not the parameterized 5 pin opamp) then all you have to do is change the name shown on the symbol in the schematic to LM356EE. The references to super menu are for an earlier version of EasyEDA. A lot of the references haven't caught up yet. Look under the "Tools" heading to run a simple or just do CTRL+R.

Stupid Autocorrupt... "Look under the "Tools" heading to run a **sim** or just do CTRL+R."

Place one of these in your schematic:  then double left click on the name to change it from UA741 to LM356EE: 

@andyfierman Thanks a bunch Andy.  We actually found a .subckt model for the  LF356, made our own spice symbol, added the found model text, and got it working.  The tricks are making sure the name of the spice symbol matches the name in the model (LF356_NS below) and the pin specification for the spice pins,  We kept trying to use the same pins numbers as in the model (like 28 and 99), but what one needs to specify is just the order they are listed in the model.  So if your model shows this: \* connections:             non\-inverting input \*                                   \|   inverting input \*                                   \|    \|   positive power supply \*                                   \|    \|    \|   negative power supply \*                                   \|    \|    \|    \|   output \*                                   \|    \|    \|    \|      \| \*                                   \|    \|    \|    \|      \| .SUBCKT LF356_NS  1   2  99  50  28 for your pin 7on the chip for the +15V  supply, it would spice pin 3 But I should do it your way to see how it compares, sounds simpler.

This is what the section 15 tries to explain in the Simulation Tutorial: [https://docs.easyeda.com/en/Simulation/Chapter15-Schematic-symbols-prefixes-and-pin-numbers/index.html](https://docs.easyeda.com/en/Simulation/Chapter15-Schematic-symbols-prefixes-and-pin-numbers/index.html) Maybe I need to clarify that for a spice symbol that calls a subckt, it is the purely the **order** of the spice pins on the spice symbol and not the name or number that must match the pin order of the subckt.

@andyfierman Maybe same something like: On the spice symbol pin map, for the spice pin number use just the number order the pins are specified in the .subckt model and not the number or letter given. And then give an example like I stated.

Actually, [https://docs.easyeda.com/en/Simulation/Chapter15-Schematic-symbols-prefixes-and-pin-numbers/index.html](https://docs.easyeda.com/en/Simulation/Chapter15-Schematic-symbols-prefixes-and-pin-numbers/index.html) does describe that it is the pin order that matters and not the names. This is explicitly shown in the section reproduced below: This can be illustrated by a simple opamp with 5 pins: inverting and non-inverting inputs; output and positive and negative supply pins but the principle applies to all spice subcircuits. The subcircuit call for this opamp might look like this in the spice netlist: > **X1 input feedback vpos vneg output opamp_ANF01** Where: > **X1** is the name of the subcircuit in the top level (i.e. the calling) circuit; > **input feedback vpos vneg output** are the netnames in the circuit calling (i.e. containing) the subcircuit and: > **opamp_ANF01** is the name of the subcircuit being called. * Pay special attention to the order of the netnames in the subcircuit call. The spice pin ordering for the majority of opamp subcircuits is like that shown in the example below: | ``` *------------------------------------------------------------------- * * opamp_ANF01 * * Simplified behavioural opamp * * Node assignments * noninverting input * | inverting input * | | positive supply * | | | negative supply * | | | | output * | | | | | * spice pin order: 1 2 3 4 5 * | | | | | .subckt opamp_ANF01 inp inn vcc vee out ; these are the netnames * used internally to the * subcircuit. B1 out 0 + V=(TANH((V(inp)-V(inn))*{Avol}*2/(V(vcc)-V(vee)))*(V(vcc)-V(vee)) + +(V(vcc)+V(vee)))/2 * .ends opamp_ANF01 * *------------------------------------------------------------------- ``` | Note that the spice pin order of the subcircuit call is in exactly the same order as that of the pins in the .subckt line of the subcircuit.