• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

LTSpice Simulation: AC Analysis showing voltage outputs way higher than power supply

Status
Not open for further replies.

eyAyXGhF

Member
Hey all,
I'm simulating a really simple circuit (op-amp driving two transistors in a push-pull configuration). When I do an AC Analysis and compare the input and output, the input looks great (10Vpp signal as I set) but the output shows a voltage going to nearly 110V!

Maybe I'm doing something wrong? I have two voltage sources, +15 and -15 connected to the net +V and -V respectively and these are the net names that I'm using on the power of the op-amp and as power where required in the circuit.

FWIW, I've set the simulation results to Bode - Linear.
 

crutschow

Well-Known Member
Most Helpful Member
The AC analysis is a linear frequency-domain analysis and assumes the circuit is linear for any voltage or current level. It pays no attention to the supply voltage, thus the output voltage can go to any value, depending only upon the gain. To see the effect of power supply voltages on the circuit signal voltages you need to do the Transient Analysis with an AC transient source.
 
Last edited:

eyAyXGhF

Member
The AC analysis is a linear frequency-domain analysis and assumes the circuit is linear for any voltage or current level. It pays no attention to the supply voltage, thus the output voltage can go to any value, depending only upon the gain. To see the effect of power supply voltages on the circuit signal voltages you need to do the Transient Analysis with an AC transient source.
Thanks for that, things look normal now.

Is there any way to do what I was achieving? That is, see the frequency response of my circuit in actual Volts? Like, have the source frequency sweep during the transient analysis?
 

eTech

Active Member
In the schematic editor, click on Simulate -> Edit Simulation cmd then click on the AC analysis tab.
You can set the parameters for a frequency sweep on the AC analysis tab.

eT
 

crutschow

Well-Known Member
Most Helpful Member
...........................................
Is there any way to do what I was achieving? That is, see the frequency response of my circuit in actual Volts? Like, have the source frequency sweep during the transient analysis?
Why do you want to do in in the transient analysis? That's what the AC Analysis is for. The best you can do in the Transient Analysis is to sweep the frequency using the SFFM source or use the .step function to change the frequency in discrete steps.
 

eyAyXGhF

Member
Why do you want to do in in the transient analysis? That's what the AC Analysis is for. The best you can do in the Transient Analysis is to sweep the frequency using the SFFM source or use the .step function to change the frequency in discrete steps.
I wanted to see the actual voltage output of the circuit across the frequencies. AC Analysis showed voltages as high as 110V, but I suppose I could just assume that any voltage shown over my power supply voltage would just result in clipping.
 

crutschow

Well-Known Member
Most Helpful Member
I wanted to see the actual voltage output of the circuit across the frequencies. AC Analysis showed voltages as high as 110V, but I suppose I could just assume that any voltage shown over my power supply voltage would just result in clipping.
Normally the actual voltages are not of concern in an AC analysis since it's just a linear simulation. But if you want to avoid voltages above the supply voltage then just use a smaller input voltage. Note, however, that if you do this any displayed dB values will still be relative to 1V.
 
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading

 
Top