Author Topic: mc34063 ltspice not simulating  (Read 2270 times)

0 Members and 1 Guest are viewing this topic.

Offline LaserTazerPhaserTopic starter

  • Regular Contributor
  • *
  • Posts: 203
  • Country: us
mc34063 ltspice not simulating
« on: January 11, 2019, 06:21:37 am »
not sure why its not simulating this boost circuit

https://nofile.io/f/mxmk6ODZVvm/27v-boost-mc34063.zip
« Last Edit: January 11, 2019, 08:03:26 am by LaserTazerPhaser »
 

Offline iMo

  • Super Contributor
  • ***
  • Posts: 5570
  • Country: va
Re: mc34063 ltspice not simulating
« Reply #1 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

Remove and insert L1 again.
Replace Diode with 1N5819.
« Last Edit: January 11, 2019, 11:21:45 am by imo »
Readers discretion is advised..
 
The following users thanked this post: LaserTazerPhaser

Offline LaserTazerPhaserTopic starter

  • Regular Contributor
  • *
  • Posts: 203
  • Country: us
Re: mc34063 ltspice not simulating
« Reply #2 on: January 11, 2019, 12:39:58 pm »
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

Remove and insert L1 again.
Replace Diode with 1N5819.

Same circuit in the screenshot results in error. The error node is the timing capacitor to IC pin.
 

Offline Ian.M

  • Super Contributor
  • ***
  • Posts: 13216
Re: mc34063 ltspice not simulating
« Reply #3 on: January 11, 2019, 01:47:03 pm »
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: [Select]
.ic V(vout)=11.5V V(vcc)=12V
It then runs OK (under LTspice IV) with default settings and no.options overrides, with a simple
Code: [Select]
.tran 100m uic
« Last Edit: January 11, 2019, 11:53:08 pm by Ian.M »
 
The following users thanked this post: LaserTazerPhaser

Offline iMo

  • Super Contributor
  • ***
  • Posts: 5570
  • Country: va
Re: mc34063 ltspice not simulating
« Reply #4 on: January 11, 2019, 02:48:19 pm »
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.
« Last Edit: January 11, 2019, 03:08:44 pm by imo »
Readers discretion is advised..
 
The following users thanked this post: LaserTazerPhaser

Offline LaserTazerPhaserTopic starter

  • Regular Contributor
  • *
  • Posts: 203
  • Country: us
Re: mc34063 ltspice not simulating
« Reply #5 on: January 11, 2019, 10:38:32 pm »
Replacing the 12v voltage source caused it to work. Apparently the voltage source built in resistance caused issues. The circuit boosts as it should.

I prefer the symbol I modified which is more accurate to the actual device pin orientation.
« Last Edit: January 11, 2019, 10:43:11 pm by LaserTazerPhaser »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf