| Electronics > Beginners |
| mc34063 ltspice not simulating |
| (1/2) > >> |
| LaserTazerPhaser:
not sure why its not simulating this boost circuit https://nofile.io/f/mxmk6ODZVvm/27v-boost-mc34063.zip |
| iMo:
Replace your ".tran 1" with this in your schematics --- Quote ---.options Gmin=1e-9 method=Gear .tran 0 100m 1u 100n uic .inc MC34063.lib --- End quote --- Remove and insert L1 again. Replace Diode with 1N5819. |
| LaserTazerPhaser:
--- Quote from: imo on January 11, 2019, 10:57:04 am ---Replace your ".tran 1" with this in your schematics --- Quote ---.options Gmin=1e-9 method=Gear .tran 0 100m 1u 100n uic .inc MC34063.lib --- End quote --- Remove and insert L1 again. Replace Diode with 1N5819. --- End quote --- Same circuit in the screenshot results in error. The error node is the timing capacitor to IC pin. |
| Ian.M:
Who in their right mind hides component designators in a sim? You don't need the .inc MC34063.lib as that's built into the symbol. It looks like the MC34063 model has a problem. If you don't use the .tran startup or uic options the operating point analysis at the beginning of the .tran run can leave it stalled in a non-oscillating steady state. There are other models in the .lib file that may be worth trying - edit U2's value (currently MC34063) to select them. Choosing a realistic model for the diode (e.g. 1N5819) helps with timestep problems as does setting initial conditions for the two big capacitors so the massive initial charging current surges aren't included in the sim. Label the Vcc node, then use: --- Code: ---.ic V(vout)=11.5V V(vcc)=12V --- End code --- It then runs OK (under LTspice IV) with default settings and no.options overrides, with a simple --- Code: ---.tran 100m uic --- End code --- |
| iMo:
Download the source from my post above. It should work fine. It could be I've been using a different symbol. Below from the downloaded .zip :-+ PS: I've been using Rsc=0.22ohm in my simul, it works fine with your 1.75ohm as well. |
| Navigation |
| Message Index |
| Next page |