You have run a .op SPICE Analysis on a circuit containing at least one voltage source, V1 and a subcircuit, XT1, containing a voltage source, VM. Both voltage sources have no DC parameter explicitly set. For more on how to set up spice Analyses voltage sources please see the EasyEDA Simulation eBook.

BTW, None of what you have reported is a bug. It is the normal response of the simulator to running a .op spice analysis. The two warnings about the DC values of the voltage sources are just that: they are warnings informing you that the explicit DC parameter has not been set. * There is nothing wrong with not setting this DC parameter. For example, suppose you wish to set up a voltage as a fixed, (time invariant) 5V supply, this is what the voltage source would look like in the spice netlist: `Vsupply VCC GND 5` If you run an analysis then ngspice (the underlying spice engine used by EasyEDA) will report: `Warning: vsupply: no DC value, transient time 0 value used` which means that at the start of a `.tran` transient Analysis (i.e. at transient time 0), and for a `.op` or for a `.ac` spice anaylsis, the value `5` will be assumed to be the value that you wish to be used. If you add `DC` to the voltage source parameters like this: `Vsupply VCC GND DC 5` then the warning will disappear. Suppose you want to ramp the voltage up from zero to 5V over a period of 1ms. Then you could configure a `PULSE()` voltage source like this: `Vsupply VCC GND PULSE(0 5 0 1m)` That will also give: `Warning: vsupply: no DC value, transient time 0 value used` but appending `DC 5` like this: `Vsupply VCC GND PULSE(0 5 0 1m) DC 5` will define a voltage source that ramps up from 0 to 5V for a `.tran` analysis but is set to a constant 5V DC for all other spice analyses. This will not give a warning. **Why do this?** The explicit `DC` parameter allows you to set up different initial conditions for transient and for other analyses. If you run a `.op` or a `.ac` analysis with a voltage source set up like this: `Vsupply VCC GND PULSE(0 5 0 1m)` then these analyses will take the the voltage at the start of the analysis to be the transient time 0 value of 0V. If you are using Vsupply to power an amplifier then your `.op` anaylsis will return 0V from everywhere in the circuit because the supply will be set to 0V! Similarly, if you run a `.ac` analysis then the gain will be zero (very large negative dB). However, if you run a `.op` or a `.ac` analysis with a voltage source set up with the extra DC parameter in it like this: `Vsupply VCC GND PULSE(0 5 0 1m) DC 5` then these analyses will take the the voltage at the start of the analysis to be DC value of %V. If you are using Vsupply to power an amplifier then your `.op` anaylsis will return the expected bias voltages from everywhere in the circuit because the supply will be set to 5V. Similarly, if you run a `.ac` analysis then the gain will be at the expected value for that circuit when powered by 5V. * For information about simulation in EasyEDA please the **EasyEDA Simulation eBook** at: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub * To select and edit the parameters in the spice independent sources, please see: https://easyeda.com/forum/topic/Selecting_Sources_in_EasyEDA-oASM4mEyQ * To understand and configure the parameters in the spice independent sources please see the **EasyEDA Simulation eBook** at: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub In particular: **Configuring Voltage and Current Sources**: https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub#h.2p2csry and: **Setting up Analyses** https://docs.google.com/document/u/1/d/1OWZVVFRAe_2NW3WratpkA_SGuHa5AcRow5ZRfvcoVTU/pub#h.3fwokq0 (The Google links above are to the original copy of the Simulation eBook which you can also find at: https://easyeda.com/Doc/Simulation-eBook/ but the table of contents in the EasyEDA copy is broken and misses out some sections. We are working to fix it but in the meanwhile the copy published to the web from Google Drive works just as well.) * There is also more about voltage sources (and everything else!) here: http://ngspice.sourceforge.net/docs/ngspice-manual.pdf#section.4.1

Thanks Andy