how to plot open-loop gain vs frequency

Status
Not open for further replies.
C

cjupiter

Member level 2
Joined
May 10, 2004
Messages
45
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,286
Activity points
430
Im not sure how to plot the open-loop gain of my opamp in spice. I want it so i have the gain in decibels on y-axis and log frequency on the x-axis. Do i have to configure my circuit in order to achieve correct plot?
 

If you have no feedback from output to input in your simulation circuit no need to change anything.
 

Add a Big RI(1G or so) between output and input, then simulate.
plot with db
 

cjupiter said:
Im not sure how to plot the open-loop gain of my opamp in spice. I want it so i have the gain in decibels on y-axis and log frequency on the x-axis. Do i have to configure my circuit in order to achieve correct plot?
Click to expand...

I'm not very sure about what's the matter with you. If the problem is about the simulation tool, providing the tool name your are using may be helpful. In hspice, you may get the gain vs. frequency curve by ac analysis and a probe statement like this:
.probe ac gain=vdb(out)

If the problem is about circuit configuration, a feedback network may or may not be needed to set the opamp's operating point. In hspice, you may set the AC resistance different from DC value for a resistor. Thus, a feedback network can be constructed to set the DC operting point of the op amp while the opamp is almost 'OPEN-CIRCIRT' in AC analysis.
 

Thanks for all the feedback everyone. I have plotted the gain by doing a frequency sweep and plotted Vout in db. I have a result but im pretty sure it is wrong. My response is in the negative decibel range instead of the positive range. I have a flat response across - 60dB and then it drops off steeply after 1MHz, becoming more negative. Is there a common reason for this?
 

Maybe your op amp didn't work with proper DC operting point. You may check the operating of each active devices. If this is the case, you may try to use the attached configuration to do a frequency sweep. The inductor and capacitor should have a large enough value.
 

    C

    cjupiter

    Points: 2
    Helpful Answer Positive Rating
I think that u have sth. wrong with your circuit.
Every problem must have a more simple than it , need be solved.
 

which tool do you use?
when i use spectre,it's easily to plot the bode curves in the direct plot fuction.
 

devrimaksin said:
Instead of an inductor put a resistor
this way you can simulate
DC gain also
Click to expand...
Inductor (very high value) will be the better choice..
If u use resistor, u need to be careful..It may cause a false information of 1st pole in ur o/p response..
I hav also seen a T-network(RCR) been used in feedback..but never tried..
Regards
 

Pls check if any transistor is in cutoff with .op command. If your circuit is OK, then you can compare the AC analysis gain with that obtained from transient anlaysis for comparison in order to make sure that your AC analysis method is correct.

Thanks
 

maybe the DC bias is wrong
 

yakyao said:
maybe the DC bias is wrong
Click to expand...

So youre saying i should bias my input transistors first with a DC source before performing the AC frequency sweep?

Thanks
 

It may or may not be a DC source. If you use a transient function (such as SIN, PWL, PULSE), the value at time 0 is used for calculate the operating point (DC bias).
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…