0
\$\begingroup\$

I'm busy simulating a Hartley oscillator that I have designed for a 64.5kHz oscillation frequency. I first simulated in LTSpice and obtained the results below which I am happy with:

LTSpice circuit LTSpice time LTSpice frequency

LTSpice unfortunately doesn't have the opamp that I want to use in practice, the TL074CN, so I am now trying to simulate in OrCad using this opamp. For some reason I cannot get the same result in OrCad as in LTSpice. I've spent hours trying to get it to work in OrCad but to no avail. I have added my OrCad schematic and the result below:

OrCad schematic OrCad time

In OrCad after my initial pulse to get oscillations going the oscillation dies out very quickly. I am at a loss as to what I am doing wrong and how the circuit seems to work in LTSpice but not OrCad. Any help would be appreciated.

\$\endgroup\$
  • \$\begingroup\$ What about the polarity of V7? \$\endgroup\$ – LvW May 13 '18 at 16:39
  • \$\begingroup\$ Have you tried with uic in OrCAD? I don't know where the setting is, though, I don't have OrCAD. Or try a different opamp, the TL has JFET inputs, IIRC. @LvW Looking at the values they seem to be fine, +5 and -5. \$\endgroup\$ – a concerned citizen May 13 '18 at 16:45
  • 2
    \$\begingroup\$ Why don't you download the model for the tl074? electronics.stackexchange.com/questions/213422/… . Plus: youtube.com/watch?v=1zUtJ0XWpaQ \$\endgroup\$ – Sredni Vashtar May 13 '18 at 16:53
  • 1
    \$\begingroup\$ Maybe the initial "noise floor" (kick) is too short for the OrCAD simulator? \$\endgroup\$ – Ale..chenski May 13 '18 at 17:12
  • 1
    \$\begingroup\$ Sometimes you have to tweak R2 so try it at 50 ohms or 100 ohms. \$\endgroup\$ – Andy aka May 13 '18 at 20:03
4
\$\begingroup\$

The spice model is available from the TI web site for the part:

* TL074 OPERATIONAL AMPLIFIER "MACROMODEL" SUBCIRCUIT
* CREATED USING PARTS RELEASE 4.01 ON 06/16/89 AT 13:08
* (REV N/A)      SUPPLY VOLTAGE: +/-15V
* CONNECTIONS:   NON-INVERTING INPUT
*                | INVERTING INPUT
*                | | POSITIVE POWER SUPPLY
*                | | | NEGATIVE POWER SUPPLY
*                | | | | OUTPUT
*                | | | | |
.SUBCKT TL074    1 2 3 4 5
*
  C1   11 12 3.498E-12
  C2    6  7 15.00E-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 4.715E6 -5E6 5E6 5E6 -5E6
  GA    6  0 11 12 282.8E-6
  GCM   0  6 10 99 8.942E-9
  ISS   3 10 DC 195.0E-6
  HLIM 90  0 VLIM 1K
  J1   11  2 10 JX
  J2   12  1 10 JX
  R2    6  9 100.0E3
  RD1   4 11 3.536E3
  RD2   4 12 3.536E3
  RO1   8  5 150
  RO2   7 99 150
  RP    3  4 2.143E3
  RSS  10 99 1.026E6
  VB    9  0 DC 0
  VC    3 53 DC 2.200
  VE   54  4 DC 2.200
  VLIM  7  8 DC 0
  VLP  91  0 DC 25
  VLN   0 92 DC 25
.MODEL DX D(IS=800.0E-18)
.MODEL JX PJF(IS=15.00E-12 BETA=270.1E-6 VTO=-1)
.ENDS

You can use that in LTSpice. If you want to just be simple about it, click on the schematic to make sure it is active and type the letter S and you will get a spice dialog. Paste the above model into that and then put it onto the schematic. Go into the opamps sections (using F2 and selecting the opamp folder) and scroll to the end of the list to see "opamp2" as a selection. Grab that and put it on the schematic. Carefully hover over the word "opamp2" on the symbol and right-click that name. A dialog showing "opamp2" in a box will pop up. Change it to TL074 and hit ENTER.

Use that symbol.

Your circuit will simulate similarly, I believe.


I don't use ORCAD and do not have access to it, so I can't help on that score. It's likely that there are some simulation controls you need to adjust to help it out in finding a solution. It could be that it is selecting a poor choice for the simulation step time, for example. But there are a number of other options in spice that could affect the outcome, too.

Here is what I got from LTspice:

enter image description here enter image description here

\$\endgroup\$
  • 1
    \$\begingroup\$ +10 Great instructions. Importing models into LTspice was always tricky for me. \$\endgroup\$ – Ale..chenski May 13 '18 at 19:47

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.