Problem with "virtual" potential in PSpice

Status
Not open for further replies.
D

Dante1555

Newbie level 4
Joined
Jul 28, 2016
Messages
5
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
40
Hello everybody. I have problem with correct simulation of OpAmp in OrCAD PSpice. In scheme on picture bellow i have "zero" potentianl and "virtual" potential for my OpAmp, which is higer than "zero" for 27v, but due internal structure of OpAmp subcircuit, its output voltage source have one terminal always connected to "zero" and scheme doesnt work as intended. is it possible to get around this limitation, add a second zero potential for example?
 

Why are you using OP07 as comparator? Presumed your observation is correct, there are hundreds of better suited OPs and comparator ICs, e.g. providing rail-to-rail output voltage which is strongly recommended for the gate driver application.
 

FvM said:
Why are you using OP07 as comparator? Presumed your observation is correct, there are hundreds of better suited OPs and comparator ICs, e.g. providing rail-to-rail output voltage which is strongly recommended for the gate driver application.
Click to expand...

Thanks for reply, but I used OP-07 for example, this OP It is the first thing that occured to me. Most models of OpAmp's in PSpice have same structure with voltage source, always connected to "zero", but some task require "virtual" potential.
 

I can confirm that the macro models with internal ground reference are effectively useless if the superimposed voltage changes dynamically. DC offsets however don't disturb the OP operation with the models that I know. The problem in your design is probably not related to internal ground reference.

There are however OP models that don't use an internal ground reference.
 
Thanks for reply. I'll rethink my design.
 

Hi,

but due internal structure of OpAmp subcircuit, its output voltage source have one terminal always connected to "zero"
Click to expand...

I don´t agree.
Many OPAMP circuits use GND, but it never is connected to GND. (No internal and no external conecction of any OPAMP pin)
For example a typical non_inverting amplifier.
--> No input, no power supply no output is connected to GND. And thus the OPAMP doesn´t know anything about GND.

****
To your circuit.
You may connect a voltmeter (or a LED) to the OPAMP output.
and you may connect the other voltmeter input to any other voltage (GND, +5V, +13V, -27V...)
--> the voltmeter will always show different values, but the OPAMP output doesn´t change.

What I want to say:
* There is no OPAMP INTERNAL connection to GND.
* It has one single output pin
* and its on you to wich voltage you decide to refer the output voltage. (or the load)

***
You connected -Supply of the OPAMP to GND.
If you want the OPAMP output to go negative, you need to connect the -Supply pin to an even more negative voltage.
In your case you can connect -Supply to -27V. (as long as the total supply voltage is in the specified range)
And again this doesn´t change output voltage when the output is positive.

But before it was impossible for the output to go negative... now it is possible to go negative.


Klaus
 
The thread is about SPICE models. TI OP07 and many other OP macro models are in fact referencing the global ground node internally. This can cause unexpected simulation errors at least if the difference voltage between global ground and local ground (e.g. V-) is changing dynamically.

Code: 
* OP-07C OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 04/06/89 AT 09:13
* (REV N/A)      SUPPLY VOLTAGE: +/-15V
* CONNECTIONS:   NON-INVERTING INPUT
*                | INVERTING INPUT
*                | | POSITIVE POWER SUPPLY
*                | | | NEGATIVE POWER SUPPLY
*                | | | | OUTPUT
*                | | | | |
.SUBCKT OP-07C   1 2 3 4 5
*
  C1   11 12 2.887E-12
  C2    6  7 30.00E-12
  DC    5 53 DX
  DE   54  5 DX
  DLP  90 91 DX
  DLN  92 90 DX
  DP    4  3 DX
  EGND 99  [COLOR="#FF0000"]0[/COLOR] POLY(2) (3,[COLOR="#FF0000"]0[/COLOR]) (4,[COLOR="#FF0000"]0[/COLOR]) 0 .5 .5
  FB    7 99 POLY(5) VB VC VE VLP VLN 0 147.3E6 -100E6 100E6 100E6 -100E6
  GA    6 [COLOR="#FF0000"] 0[/COLOR] 11 12 113.1E-6
  GCM   [COLOR="#FF0000"]0[/COLOR]  6 10 99 56.69E-12
  IEE  10  4 DC 7.501E-6
  HLIM 90  [COLOR="#FF0000"]0[/COLOR] VLIM 1K
  Q1   11  2 13 QX
  Q2   12  1 14 QX
  R2    6  9 100.0E3
  RC1   3 11 8.841E3
  RC2   3 12 8.841E3
  RE1  13 10 1.943E3
  RE2  14 10 1.943E3
  REE  10 99 26.66E6
  RO1   8  5 30
  RO2   7 99 30
  RP    3  4 12.04E3
  VB    9  [COLOR="#FF0000"]0[/COLOR] DC 0
  VC    3 53 DC 2.900
  VE   54  4 DC 2.900
  VLIM  7  8 DC 0
  VLP  91  [COLOR="#FF0000"]0[/COLOR] DC 20
  VLN   [COLOR="#FF0000"]0[/COLOR] 92 DC 20
.MODEL DX D(IS=800.0E-18)
.MODEL QX NPN(IS=800.0E-18 BF=5.357E3)
.ENDS
 
Hi,

I have to admit, that i forgot that this is only about models.

My post was about true circuits, so it may be useless here.

Klaus
 


Here,is what I was talking about. The first thing that occurred to me, is make new OP from existing OP subcircuit, but with addition of new ground terminal instead of "zero" terminal. Rebuild a large number of subcircuits I find irrational, and therefore interested in whether there are options for add a second ground or else to solve this problem.
 

As far as I'm aware of, there's no option to substitute node 0 in subcircuits.

But as previously mentioned, I don't see a problem with constant offset between global ground and power supply terminals.
 

FvM said:
As far as I'm aware of, there's no option to substitute node 0 in subcircuits.
Click to expand...
This can be solved very simply. You can copy all text from reference subcircuit, create new component, rename all "0" to any title, in line with name's of terminal add new title. Further you must create new symbol lib (.olb) and rewraw looks like OP, but with new additional termianl.

FvM said:
But as previously mentioned, I don't see a problem with constant offset between global ground and power supply terminals.
Click to expand...

as I had said earlier , if we look at scheme, 13 < 27 and MOSFET will always be closed. I do not argue, in reality, this scheme will work without problems, but problem in modeling, not exactly a problem, but a significant inconvenience.
 

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…