Hi Clamb09, Welcome to EasyEDA. There are a couple of simulation mistakes in your circuit: 1. You need to make V1 ramp up from 0V; 2. You have named the ground symbol connected to V2 on the lower left of the schematic, `GND1`. Spice does not understand that this is a ground when you do that. `GND1` is just a netlabel like any other whereas `GND` or `0` has the special (and reserved) meaning of `ground`; 3. As a consequence of (2), the loads to each 555 timer are floating and so cause a convergence failure because there is no proper return path to the real ground on the lower right hand side of the schematic. 4. You have chosen the LEDs from the EasyEDA Libs which from EasyEDA version 4.1 no longer have simulation models associated with them. Please see: https://easyeda.com/forum/topic/How_to_find_simulatable_parts_in_EasyEDA-1YgasK2kC Points (1) to (3) are all explained in the EasyEDA Simulation eBook. You have made a philosophical mistake in trying to get a big simulation working before you have got the basic elements of it working. In simulation it is best to start small and build up to a bigger simulation. First get one 555 timer section working. Then add the LED driver components. Then replicate those sections as required. You have also made a couple of electronics design mistakes. 1. It is bad practice to drive the base of a common emitter connected a bipolar transistor directly from a low impedance voltage source (which is what the 555 timer output looks like). You must have a resistor in series with the base. The way you have connected the 2N3904 transistors would be OK if they were replaced by N channel MOSFETs but it will not work with BJTs. 2. V2 is set to 99V. This is way over the max Vce rating of the 2N3904: http://web.mit.edu/6.301/www/2N3904o.pdf :)