Your 555 symbol has no spice model associated with it. Please see: https://easyeda.com/forum/topic/How_to_find_simulatable_parts_and_run_a_simulation_in_EasyEDA-1YgasK2kC Please then read the Simulation eBook as advised. With a 555 timer, you will also need to use one of the techniques described in the section on `Initial Conditions and starting up circuits`. You will not get a squarewave out of the 555 timer the way you are trying to. It is simply not possible. You need to use a circuit like this: https://easyeda.com/andyfierman/Variable_duty_cycle_fixed_frequency_555_oscillator-1bc9b3f6a8cf4b3c88e5f22f6780f9c6 and adjust the pot for 50% duty cycle. For the care and feeding of a real 555 timer please also see: https://easyeda.com/andyfierman/Power_supply_decoupling_and_why_it_matters_-451e18a0d36b4f208394b2a2ff7642c9 A much simpler way to get a more exact sqaurewave is shown in: https://easyeda.com/andyfierman/How_to_use_EasyEDA_Schmitt_Trigger_input_logic_gates_as_an_oscillator-lSQqYPXR9 or a more copmplex way but one which - by using the triangle wave output - requires far less filtering: https://easyeda.com/andyfierman/How_to_use_EasyEDA_Schmitt_Trigger_input_logic_gates_as_an_oscillator-lSQqYPXR9 :)

Andy, I'm drinking from a fire hose! My problem is much more basic! I start at 'Parts' -> 'System Components' ->and highlight 'Spice Simulation', then type 555 in the search window and click the 'Search' button. Search returns a long list of items containing 555. I have no clue how to find the one that was contained in 'Spice Simulation'. I know it is 'operator error', but I can't figure out how to easily find the 555 in the 'Spice Simulation' section. If I have 'Spice Simulation' highlighted and use Control F, the search finds (highlights) all the previous items found when I clicked the 'Search' button. Do I have to manually scroll through all of the 'Spice Simulation' subsections to locate the 555? The webpage you linked makes it 'sound' easy?? But I'm hard of hearing! BTW, I can generate square waves using a 555. I believe you intended to say 'Sine'. Can you try running my project? I still can't get it to run in the simulator using the BJT model 555. Sorry for being so old, slow, and stupid. Garry

Hi Garry, In your schematic (as forked at 170103 19:27 GMT) you have a DIP switch which has no simulatable model and a LED that has no simulatable model. For simulation purposes, 1. Replace the switch with a wire; 2. the LED can be replaced with Dledy, Dledr, Dledg or Dledo from the Spice Discrete section. Your simulation results show: `doAnalyses: Too many iterations without convergence` This is because you have not put in any of the techniques that you need to use to kick-start simulation circuits like the 555 astable. Change the voltage of V1 from `12` to `PULSE(0 12)` to generate a 0V to 12V supply step at T=0. The next problem is that you have accidentally placed `volprobe1` on the drawn 'lead' of the LED so it is not connected into the schematic. Volprobes must be connected to wires or directly to component pins and should therefore have a little red join dot at their probing ends. Lastly, your simulation analysis statement has way too high a max timestep. If you look in the spice netlist `Document > Miscellaneous > Simulate > Simulation Results > Download netlist` you'll find there's a line that goes: `tran 100 10s 0` Your `Max timestep` needs to be about (Stop time)/1000 i.e. 10m. This will show up in the netlist as: `tran 10m 10s 0` Then your sim will run. :) BTW: If you do the sums; https://en.wikipedia.org/wiki/555_timer_IC you will see that you can never achieve a 50% duty cycle using the form of astable that you have simulated. You can get close to it by making R3 << R1 (using your circuit prefixes) but it will never be exact.

`I'm drinking from a fire hose!` Yes, the spice component search still needs improvement. If you go to the web-based or pdf list of available parts, you can search that then copy and paste the part into the SHIFT+F search. Simulation is not easy. We have tried to make it easier but it is still about an order of magnitude harder to get to grips with than the rest of the Schematic Capture and PCB Design tools. There are so many (mostly not very intuitive) aspects of simulation. Things like the way switches can leak charge onto capacitors in a way that real switches *appear* not to. You have to think very hard about what *really* happens in the real world to make sense of some of the things that seem crazy about simulations. :) That's why we stress reading and playing with the examples in the Simulation eBook before trying any simulation work. Anyhow, you should be running now?