LTSpice showing different output DC with same circuit

Status
Not open for further replies.

Willen

Well-Known Member
Hi,
I don't know what the LTspice trying to show me. In Transient, if I set 2 second stop time, the osc (voltage booster) showing nothing boosted (just showing around 8V which is its supply voltage). If I set 2 mili-second stop time without changing any parts then I can see the boosted output of more than 20 volts. WHAT I should understand ?

(I made the osc in real world. When I measured output with my DMM, it whows 18V just first half a second then starts to show 8V. Maybe it has high impedance output which cannot drive my DMM?)
 

Attachments

  • MXL990 mic OSC.asc
    2.1 KB · Views: 292
You've run into a common problem with oscillator simulations.
Circuits with oscillators sometime will not start or start erratically in simulation, since the circuit normally does a DC analysis at the start, and this can put the oscillator in a quasi-stable, non-oscillatory state with no intrinsic noise to start it.
Check the voltage startup at 0V box or the Skip initial operating point box in the transient analysis which eliminates the initial DC analysis and usually starts the oscillator.



Don't know why the voltage drops that much with your meter attached.
 
Last edited:
since i don't have LTspice on my work computer, i went and found a schematic for one of these microphones [here].
if you are measuring at the element, the oscillator/rectifier voltage is being sourced through a 1G resistor. at least that's according to that schematic. your DMM has an input resistance of 10M. the condenser element only needs an electrostatic charge on it, so there's barely any charging current from the oscillator/rectifier. it's entirely possible the 10M input resistance of the DMM is loading the circuit down.
 
Hi, Thank you! It worked! But with 2 second stop time, it took me tens of minutes to simulate 100%. Is it normal?

I was thinking same, but a member here who donated me the MXL mic said he measured 40V output (after 1Meg resistor or across filter cap) on his DMM. My DIY condenser mic has little lower gain so I am thinking that I made a faulty OSC...
 
Willen said:
But with 2 second stop time, it took me tens of minutes to simulate 100%. Is it normal?
Click to expand...
Yes.
Simulating a high frequency circuit for a long period of time requires a zillion (estimate) calculations which takes a lot of time, even with a modern PC.
My laptop takes about a minute to do 2ms of simulation, so 2 seconds sim time would take about 17 minutes real time.

I measured an oscillator frequency of about 1MHz so for 2s, that's 2 million cycles.
So it calculates about 33 oscillator cycles per real-time second.
And each cycle takes many floating-point calculations.
 
Status
Not open for further replies.

Similar threads

R
  • Question
LTSPICE simulation of AC/DC converter
Replies
11
Views
10K
srilatha
S
LTSpice initial conditions help, please?
Replies
14
Views
2K
rjenkinsgb
F
  • Question
How to get Triac LTspice sim working?
Replies
2
Views
3K
Flyback
F
F
  • Question
Checking Altium PCBs are the same
Replies
5
Views
6K
ChrisP58
F
  • Question
LTspice...Mouse disappears
Replies
1
Views
8K
eTech
E
Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…