LM833 bandwidth problem

Guest
I'm simulating an LM833 in inverting mode, very simple. just the two
resistors. And according to all datasheets the GBP of this amplifier is
typicaly 15 Mhz. This means that in the circuit of my amplifier, that
has two resistors of 10K, the gain is 1, so the bandwidth of my circuit
is half the GBP (correct me if i'm wrong, i'm new in this stuff). Why
the simulation in pspice show me that pole in 9Mhz??
Did anyone had the same problem?
 
<toto.mongui@gmail.com> schrieb im Newsbeitrag news:1155782309.720893.253160@75g2000cwc.googlegroups.com...
I'm simulating an LM833 in inverting mode, very simple. just the two
resistors. And according to all datasheets the GBP of this amplifier is
typicaly 15 Mhz. This means that in the circuit of my amplifier, that
has two resistors of 10K, the gain is 1, so the bandwidth of my circuit
is half the GBP (correct me if i'm wrong, i'm new in this stuff). Why
the simulation in pspice show me that pole in 9Mhz??
Did anyone had the same problem?
Click to expand...

Hello toto,

This is a good question.

I have only the model from ONSEMI. Their model has a GBW of
about 13MHz calculated from a measured/simulated open loop
frequency rsponse at 100kHz. The open loop unity gain frequency
is 10Mhz in the LM833 model from ONSEMI's webpage.

Don't rely on the datasheet here. You should measure GBW of your
model before you try with the theory.

My model gives a -3B-bandwidth of 9Mhz for a gain of 2 or -1.
From the theory we would expect a BW between 5MHz and 6.5MHz
for this gain setting.

What theory do we have in mind?

Fc = GBW/gain Fc=-3dB corner frequency

This theoretical model assumes a perfect 90 degree phase shift
of the open loop gain. Do we have that in our LM833 SPICE model?
The answer is no! We have phase a shift of about 128degree
at 10MHz (0dB gain). The SPICE model and the real opamp are
at least a second order system whereas the theoretical model
is based on a first order model.
Now choose a gain of 100. Here we have 90dgree phase shift
in our SPICE model too. The simulaton gives a banwidth of
about 130kHz. This is a good match with the theory. (13Mhz/100)
Summary: We can use the the therotical formula for bandwith
calculation only up to a frequency of about 1/10 of GBW,
because the phase shift is increasing for higher frequencies.

I have to admit that I never thought about that before, because
opamps are normally never used so close to their GBW. GBW is a
very weak specified parameter. It may vary from 10MHz to 20MHz
from part to part for the LM833. Be aware that the opamps from
all manufacturers have a large tolerance of their GBW.


Best regards,
Helmut

I have simulated with LTspice.
http://www.linear.com/designtools/softwareRegistration.jsp

http://groups.yahoo.com/group/LTspice/
 
Thak you Hetmul, that was very useful. I'm taking a course in college
of design with operational amplifiers, and the idea of the first lab is
to push the model to it's limits, and books normally avoid this kind of
problems.
Helmut Sennewald ha escrito:

toto.mongui@gmail.com> schrieb im Newsbeitrag news:1155782309.720893.253160@75g2000cwc.googlegroups.com...
I'm simulating an LM833 in inverting mode, very simple. just the two
resistors. And according to all datasheets the GBP of this amplifier is
typicaly 15 Mhz. This means that in the circuit of my amplifier, that
has two resistors of 10K, the gain is 1, so the bandwidth of my circuit
is half the GBP (correct me if i'm wrong, i'm new in this stuff). Why
the simulation in pspice show me that pole in 9Mhz??
Did anyone had the same problem?


Hello toto,

This is a good question.

I have only the model from ONSEMI. Their model has a GBW of
about 13MHz calculated from a measured/simulated open loop
frequency rsponse at 100kHz. The open loop unity gain frequency
is 10Mhz in the LM833 model from ONSEMI's webpage.

Don't rely on the datasheet here. You should measure GBW of your
model before you try with the theory.

My model gives a -3B-bandwidth of 9Mhz for a gain of 2 or -1.
From the theory we would expect a BW between 5MHz and 6.5MHz
for this gain setting.

What theory do we have in mind?

Fc = GBW/gain Fc=-3dB corner frequency

This theoretical model assumes a perfect 90 degree phase shift
of the open loop gain. Do we have that in our LM833 SPICE model?
The answer is no! We have phase a shift of about 128degree
at 10MHz (0dB gain). The SPICE model and the real opamp are
at least a second order system whereas the theoretical model
is based on a first order model.
Now choose a gain of 100. Here we have 90dgree phase shift
in our SPICE model too. The simulaton gives a banwidth of
about 130kHz. This is a good match with the theory. (13Mhz/100)
Summary: We can use the the therotical formula for bandwith
calculation only up to a frequency of about 1/10 of GBW,
because the phase shift is increasing for higher frequencies.

I have to admit that I never thought about that before, because
opamps are normally never used so close to their GBW. GBW is a
very weak specified parameter. It may vary from 10MHz to 20MHz
from part to part for the LM833. Be aware that the opamps from
all manufacturers have a large tolerance of their GBW.


Best regards,
Helmut

I have simulated with LTspice.
http://www.linear.com/designtools/softwareRegistration.jsp

http://groups.yahoo.com/group/LTspice/
Click to expand...
 
Hello Toto,

thanks for your feedback. Could you please forward my answer to
your teacher and other course attendees too. Maybe they also have
never thought about that as I did in the past.
Does anybody in this course know LTspice?

Best regards,
Helmut

"Toto" <toto.mongui@gmail.com> schrieb im Newsbeitrag news:1155863045.710039.19010@m79g2000cwm.googlegroups.com...
Thak you Hetmul, that was very useful. I'm taking a course in college
of design with operational amplifiers, and the idea of the first lab is
to push the model to it's limits, and books normally avoid this kind of
problems.
Helmut Sennewald ha escrito:

toto.mongui@gmail.com> schrieb im Newsbeitrag news:1155782309.720893.253160@75g2000cwc.googlegroups.com...
I'm simulating an LM833 in inverting mode, very simple. just the two
resistors. And according to all datasheets the GBP of this amplifier is
typicaly 15 Mhz. This means that in the circuit of my amplifier, that
has two resistors of 10K, the gain is 1, so the bandwidth of my circuit
is half the GBP (correct me if i'm wrong, i'm new in this stuff). Why
the simulation in pspice show me that pole in 9Mhz??
Did anyone had the same problem?


Hello toto,

This is a good question.

I have only the model from ONSEMI. Their model has a GBW of
about 13MHz calculated from a measured/simulated open loop
frequency rsponse at 100kHz. The open loop unity gain frequency
is 10Mhz in the LM833 model from ONSEMI's webpage.

Don't rely on the datasheet here. You should measure GBW of your
model before you try with the theory.

My model gives a -3B-bandwidth of 9Mhz for a gain of 2 or -1.
From the theory we would expect a BW between 5MHz and 6.5MHz
for this gain setting.

What theory do we have in mind?

Fc = GBW/gain Fc=-3dB corner frequency

This theoretical model assumes a perfect 90 degree phase shift
of the open loop gain. Do we have that in our LM833 SPICE model?
The answer is no! We have phase a shift of about 128degree
at 10MHz (0dB gain). The SPICE model and the real opamp are
at least a second order system whereas the theoretical model
is based on a first order model.
Now choose a gain of 100. Here we have 90dgree phase shift
in our SPICE model too. The simulaton gives a banwidth of
about 130kHz. This is a good match with the theory. (13Mhz/100)
Summary: We can use the the therotical formula for bandwith
calculation only up to a frequency of about 1/10 of GBW,
because the phase shift is increasing for higher frequencies.

I have to admit that I never thought about that before, because
opamps are normally never used so close to their GBW. GBW is a
very weak specified parameter. It may vary from 10MHz to 20MHz
from part to part for the LM833. Be aware that the opamps from
all manufacturers have a large tolerance of their GBW.


Best regards,
Helmut

I have simulated with LTspice.
http://www.linear.com/designtools/softwareRegistration.jsp

http://groups.yahoo.com/group/LTspice/
Click to expand...
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top