Been trying to simulate on multisim a circuit I saw about high voltage amplifier:


Schematic source seems to be:

EDN Design Ideas, 2004 - page 123 of 155 (displayed page number 110)
High-voltage amplifier uses simplified circuit
Jui-I Tsai, Jun-Ming Shieh, Tai-Shan Liao, and
Ching-Cheng Teng, National Chiao Tung Unversity, Taiwan

There are also corrections in the comments below this original article:

EDN - High-voltage amplifier uses simplified circuit
October 14, 2004

The input is 8 Vp-p and 100Hz and reached to output of 1800 Vp-p and 100Hz. The publisher mentioned he used the following parts to build it: OP07 , LM356, MTP2P50E and BUK456800B.

In the multisim database, I couldn't find these exact parts (perhaps because companies stopped creating them). So, instead I used the following parts for the following simulation: OP07, LF356H, MTP2P50EG and NDD03N80Z-1G.


enter image description here

For input 8 Vp-p and 100Hz, I got the result of approx. 8 V: enter image description here

And I can't figure out whats the problem with the design I implanted on the multisim, as I don't get the high voltage that is desired. Thank you for anyone who reads this and tries to help me, much appriciated !

  • 1
    \$\begingroup\$ Have you tried it at DC or very low frequency? With those very high gate resistors and no compensating capacitors, it won't work very fast. \$\endgroup\$ Commented Sep 15, 2020 at 13:54
  • \$\begingroup\$ @KevinWhite I just tried switching to low frequency and then with DC, but no promising results, unfortunately. \$\endgroup\$ Commented Sep 15, 2020 at 14:10
  • 1
    \$\begingroup\$ Your PMOS connections are wrong. In the original, sources to the top, drains to the bottom. In yours, sources to the bottom, drains to the top. \$\endgroup\$ Commented Sep 15, 2020 at 14:19
  • \$\begingroup\$ @RohatKılıç I noticed that in the original paper as well before, tried to connect them as he did, yet it still doesn't work properly. \$\endgroup\$ Commented Sep 15, 2020 at 14:26
  • \$\begingroup\$ Looks like some of those "dot" connection points are mis-placed, so badly that the circuitry intention is not immediately apparent. \$\endgroup\$
    – glen_geek
    Commented Sep 15, 2020 at 16:05

1 Answer 1


I found some errors in the original schematic, they are corrected. eredeti

For newer FETs, the quiescent current had to be set. I set this to 5mA with R19 and R25. (14k instead of 10k.) There is no point in looking in front of the LF356, there is only a -2 gain there (OP07). mostemető

The DC gain is approx. 174x.

DC transfer characteristics: dctrans

At 100Hz, the gain is approx. half the DC gain. 100hz

  • \$\begingroup\$ Thank you so much for spending the time and helping me out! I will try it out. Are there any other similar components to FQD2N100 and FQD3P50? and is it possible to reach output of 1.3kV with this circuit? Thank you so much again \$\endgroup\$ Commented Sep 16, 2020 at 11:08
  • \$\begingroup\$ I liked it, so I dealt with it. :) NMOS is not a problem, there is a large selection above 600V. I did not find more than 500V from PMOS. In the first stage, they operate at half the supply voltage. The PMOS model is starting to limit at 550V. It is important that its leakage current is small at 500V because the first stage operates at 280uA (FQD3P50 has 1uA). A similar forward characteristic is required at low currents (below 5mA) for the working point to be well adjustable. If you find a minimum 700V PMOS device, it can run from 1.3kV. \$\endgroup\$
    – csabahu
    Commented Sep 16, 2020 at 14:26
  • \$\begingroup\$ Appreciate everything you have done for me! Thank you for your guidance! I got one last small question if you don't mind. What program are you using in order to build the circuits and simulations? \$\endgroup\$ Commented Sep 30, 2020 at 10:55
  • \$\begingroup\$ I just used Tina (v 9.3) now, but I have LTSpice, Tina-TI, and PSpice for TI 2020. Depending on what I want to model, I always need another one. \$\endgroup\$
    – csabahu
    Commented Sep 30, 2020 at 11:07
  • \$\begingroup\$ I see. About the Vp (Voltage peak) of the last simulation you sent, will it work with lower voltage input? for example, maximum 5Vpp? \$\endgroup\$ Commented Sep 30, 2020 at 11:34

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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