Why the signal oscillates @ 100KHz in the transient analysis?

Status
Not open for further replies.
A

AAOAA

Junior Member level 2
Junior Member level 2
Joined
Oct 31, 2013
Messages
20
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
150
Could someone please help me with this. The bode plot seems to be OK @100kHz. But I cant figure out why the signal oscillates @ 100KHz in the transient analysis?

Bode_Plot.jpg

Transient.jpg

The_circuit.jpg
 

Check your simulation circuit, you have R6 shorted out and possibly a missing ground at R3 and R4.

Brian.
 

Your circuit is missing the very important supply bypass capacitors shown and talked about in the datasheet.
So read the datasheet!
 

Thank u so much for your replys. But is the bode plot useless at this point (since the phase @ 100KHz doesnt indicate for oscillation)?
 

Missing supply bypass capacitors do not affect the phase of the input and output. It allows the output to feed into the input through the power supply.
 

AAOAA said:
Thank u so much for your replys. But is the bode plot useless at this point (since the phase @ 100KHz doesnt indicate for oscillation)?
Click to expand...

It would be interesting (better: important!) to know what your BODE plot shows. Which transfer function?
 

This is all in a simulation, right? Quite likely there is no oscillation, your simulator's just misbehaving. Try changing the minimum timestep for your transient analysis. That may solve the problem.
 

godfreyl said:
This is all in a simulation, right? Quite likely there is no oscillation, your simulator's just misbehaving. Try changing the minimum timestep for your transient analysis. That may solve the problem.
Click to expand...
I don`t think so. The time steps seem to be OK - look at the simulation results, they look smoothly. Don`t blame the simulator - in nearly 100% of all cases it is not the simulation engine but the user who shows "misbehaving".
 
In the schematic, the signal source is not connected to the circuit.
What is the input of the circuit? Is the input the line that is spelled wrong "impedence"?
 

Apart from the question if it's a reasonable circuit and if every detail is connected as intended, you obviously did not measure loop gain.

Measuring loop gain right shows about 50 dB DC gain and multiple crossings of the 0 dB line.

In the schematic, the signal source is not connected to the circuit.
Click to expand...
It is, by a behavioral expression for R3 resistance.
 
- - - Updated - - -



Actually, I got this circuit from application note of Linear Technology, with other Opamps it works well. Could you tell me please how you measured the loop gain to be 50dB?

Thanks...
http://cds.linear.com/docs/en/application-note/an43f.pdf
 
Last edited:

Loop gain can be e.g. determined by Middlebrook's method. It has been quite often discussed at Edaboard, some examples:
https://www.edaboard.com/threads/300916/
https://www.edaboard.com/threads/177993/

Regarding bridge circuit stability, the problem in this case is PSRR and it's frequency characteristic. Apart from the question, if floating supply is a good means for practical amplifier design, it's really a bad idea to implement it with a 500 MHz amplifier like LT1222. If you look thoroughly on your simulation, you'll notice that the oscillation frequency is around 80 MHz, not 100 kHz.
 

By the way capacitor bypassing of power supply in simulation is not needed because power supply impedance is 0ohm or 1mohm depends on parameters settings in simulation software.
 

Status
Not open for further replies.

Similar threads