Author Topic: Differing Response in Transient vs AC Analysis in LTSpice  (Read 1229 times)

0 Members and 1 Guest are viewing this topic.

Offline TeddyPythonTopic starter

  • Contributor
  • Posts: 36
  • Country: gb
Differing Response in Transient vs AC Analysis in LTSpice
« on: May 31, 2020, 08:01:53 pm »
I'm trying to design a HV differential probe as a project which should teach me more about op amps (so far I've only covered just simple 10's kHz amps). After some background reading, I settled on trying to achieve the following specs:

+-500V input (AC+DC)
20MHz bandwidth (-3dB)
+-5V output (100:1 attenuation)

And I've created the following circuit as a starting attempt:



With some op amps I have chosen for their high input Z, high bandwidth, and relatively low cost. When I perform an AC analysis the circuit seems to have a very flat gain with <1dB of ripple - the following says I should expect values very close to 5V up to just over 20MHz.



However, when I perform a transient simulation at 20 MHz I see the output is much smaller when compared to 5 MHz.

20MHz:



5MHz:



Why am I seeing this difference between simulation types in LTSpice? Or rather, how should I be interpreting these two different simulations? Presumably I'm not understanding the output of the AC analysis.

I've also included the schematic file for LTSpice if anyone would like them.

« Last Edit: May 31, 2020, 08:06:30 pm by TeddyPython »
 

Offline Someone

  • Super Contributor
  • ***
  • Posts: 5156
  • Country: au
    • send complaints here
Re: Differing Response in Transient vs AC Analysis in LTSpice
« Reply #1 on: May 31, 2020, 10:45:11 pm »
Depends on the opamp models, try switching them to "ideal" infinite speed devices and see if the results match.

GBW != slew rate
 
The following users thanked this post: TeddyPython

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2766
  • Country: ca
Re: Differing Response in Transient vs AC Analysis in LTSpice
« Reply #2 on: May 31, 2020, 11:24:53 pm »
TeddyPython,

Depends on the opamp models, try switching them to "ideal" infinite speed devices and see if the results match.

GBW != slew rate

+1

Here is a slightly different model:



I placed the AD817 on the schematic and used the symbol for a generic op-amp. Doing it this way it is portable.

I am stepping the Frequency so that I can both results on the same graph.

If I test at 100V peak I get a result consistent with the AC analysis.



At 500V peak it is amplitude limited. This indicates a slew rate limitation.




* eevblogprobe_JDB.asc (7.36 kB - downloaded 24 times.)

Regards,
Jay_Diddy_B

 
The following users thanked this post: TeddyPython

Offline TeddyPythonTopic starter

  • Contributor
  • Posts: 36
  • Country: gb
Re: Differing Response in Transient vs AC Analysis in LTSpice
« Reply #3 on: May 31, 2020, 11:36:10 pm »
I see, thanks both for the information.

Also thanks Jay for the tip making the schematic more portable.

I will look for a faster slew rate op amp tomorrow and report back.
 

Offline TeddyPythonTopic starter

  • Contributor
  • Posts: 36
  • Country: gb
Re: Differing Response in Transient vs AC Analysis in LTSpice
« Reply #4 on: June 01, 2020, 06:18:11 pm »
I've done some tests with a THS4631 and the result is much better, indeed gain is acceptable (to me) up to almost 25MHz at +-500V, or +-700V at 20 MHz. This did need some small capacitances though, but I was thinking these might occur from parasitics anyway, or could be added with some wires bodged over components. Alternatively, is there a better way to get a decent response without resorting to such small capacitances?



Also included another version of the spice schematic.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf