Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Making an Ideal Opamp for simulation

Status
Not open for further replies.
A

aryajur

Advanced Member level 3
Joined
Oct 23, 2004
Messages
793
Helped
124
Reputation
248
Reaction score
37
Trophy points
1,308
Location
San Jose, USA
Activity points
7,788
ideal op amp

How do I make an ideal opamp for simulation in Cadence??
I tried using the vcvs source but the output voltage of that does not clip at the set voltages !! I set the Max Output and Min Putput voltage in the properties but it simply doesn't care for them. It just shoots up !
Any suggestions would be greatly appreciated.
 

ideal op amp in cadence

The hspice model of vcvs recognizes the max and min parameters, but the spectre model does not. If you are using spectre, you may use veriloga to model the saturation effect.
 
pspice ideal opamp

you can use vcvs as a Ideal Opamp for simulation
 

vcvs cadence

How do I use veriloga?? I don't know anything about that, please help.
 

orcad ideal op amp

The vcvs in cadence does really care the saturation effect of output voltage (by max and min output voltage). While it is cared by spectre, it is ignored in SpectreS.
 
ideal opamp spice model

In Orcad Pspice there is a device name OPAMP
If you Capture CIS You Can find this Ideal Device.
Some of its characteristics are:

1- No Supply Need
2- 3 Pin Configuration (Inverting and Noninverting Input and 1 Output)
3- No Offset Pins
4- Infinity Gain with Infinity Bandwidth
 

veriloga opamp model

In Orcad Pspice there is a device name OPAMP
If you Capture CIS You Can find this Ideal Device.
Some of its characteristics are:

1- No Supply Need
2- 3 Pin Configuration (Inverting and Noninverting Input and 1 Output)
3- No Offset Pins
4- Infinity Gain with Infinity Bandwidth
 

vcvs opamp

aryajur said:
How do I use veriloga?? I don't know anything about that, please help.
Click to expand...

Here is an example for an opamp with output saturation:
Code: 
module opamp(OUT, VP, VN);
  parameter gain=10000.0;
  parameter vmax=13.0, vmin=-13.0;
  output OUT;
  electrical OUT;
  input VP;
  electrical VP;
  input VN;
  electrical VN;
  real Va;
  analog begin
    Va = gain*V(VP, VN);
    if(Va > vmax) Va = vmax;
    if(Va < vmin) Va = vmin;
    V(OUT) <+ Va;
  end
endmodule
 
orcad opamp model ideal

It is very easy to setup a ideal opamp in spectre. One vcvs source is OK. Furthermore, by adding some resistors and caps, u can model a real opamp. For example, using 2 vcvs sources 2 res and 2 caps, u can model a 2-pole opamp. Each pole is determined by a pair of res and cap, and the two pairs are separated by one vcvs source.
 
ideal ampop cadence

you can add the ahdl library into candence, then you can call the ideal opamp there to run simulation.
 

ideal op amp orcad

use clamp circuit (diode transistor) at the output.
 

idealized opamp orcad

is it possible to model slew rate effect in this VCVS based ideal opamp model.

thanks much
 

cadence ideal op amp

There is an excellent document that comes with another simulator : **broken link removed**

It uses basic blocks that are available in all simulators.
 

Hughes and Terryssw , thanks for the tip. i didnt know what the purpose of vcvs was, till i decided to dig a lil deeper.

I need to simulate an uA741 Op-amp characteristics (as an Op-amp and then with a butterworth), I have moved away from pSpice for simulating this because of some software bug during plotting.

Is there a way i can get an actual uA741 Op-amp scematic (no necessarily a layout), or is it too much to ask for? since that propietry to companies...

I managed to get an Ideal Op-Amp going for now, will await any suggestions on uA741 Op-Amp before moving back to PSpice :(
 
Last edited:

I believe that the simulation package LTPSICE from "Linear Technology" (available for free via internet) contains a model for the 741 based on transistors rather than controlled sources. (Perhaps KEITH can confirm, or not?).
In addition I know that also MICROCAP (simulatiuon package from spectrum-soft) has a transistor based model for the uA741.
 

You may find other useful simulation blocks in the "basic" and
"sample" libraries. Look for limiter functions.

Look for old web stashes of PSPICE libraries, and LTSpice
libraries, where macromodels are in plain text. The LTSpice
Yahoo! group has a really large repository of files you can
translate or patch in (you would have to sign up to get
the path I think).
 

I have [very] old Pspice libraries but the 741 models are not at the transistor level. There are plenty of "macro model" versions though. I have a circuit for the 741 with resistor values which I can post if anyone wants it, but without transistor models I doubt it will do a better job than the macromodels.

Keith.

Code: 
* connections:   non-inverting input
*                | inverting input
*                | | positive power supply
*                | | | negative power supply
*                | | | | output
*                | | | | |
.subckt uA741    1 2 3 4 5
*
  c1   11 12 8.661E-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  0 poly(2),(3,0),(4,0) 0 .5 .5
  fb    7 99 poly(5) vb vc ve vlp vln 0 10.61E6 -10E6 10E6 10E6 -10E6
  ga    6  0 11 12 188.5E-6
  gcm   0  6 10 99 5.961E-9
  iee  10  4 dc 15.16E-6
  hlim 90  0 vlim 1K
  q1   11  2 13 qx
  q2   12  1 14 qx
  r2    6  9 100.0E3
  rc1   3 11 5.305E3
  rc2   3 12 5.305E3
  re1  13 10 1.836E3
  re2  14 10 1.836E3
  ree  10 99 13.19E6
  ro1   8  5 50
  ro2   7 99 100
  rp    3  4 18.16E3
  vb    9  0 dc 0
  vc    3 53 dc 1
  ve   54  4 dc 1
  vlim  7  8 dc 0
  vlp  91  0 dc 40
  vln   0 92 dc 40
.model dx D(Is=800.0E-18 Rs=1)
.model qx NPN(Is=800.0E-18 Bf=93.75)
.ends
 
Last edited:

yes,
I have LT Spice aswell, that was my last option. My PSpice was missing some library files. Apparantly i had saved my schematic in D Drive and PSpice wasnt able to link , i assume, some of its PROBE files.

Now it is up and running again.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top