Using Transformers in circuits SOLVED

I am trying to set the transformer parameters to model a Tamura PL30-12-130B (data sheet available at According to Tamura's data sheet using the primary and secondary in series configurations, with a primary voltage of 230AC, the secondary should be capable of 12.6AC - 2.4Amps, or 30VA.
I created a simple circuit: 230V AC Source connected to the Primary side and a 5.25 ohm resistor on the secondary. Secondary at 12.6 volts (n=18.25) should be 2.4 amps, which matches the specs from Tamura. My circuit is Public here: Transformer-230-12p6

The T-D simulation provides voltages (peak primary and secondary) and peak secondary current that seem correct, however the primary current is far in excess of anything normal. For a simple step down (18.25:1) transformer like this, I would expect a Primary current of approximately 130mA RMS (or roughly 183mA peak) for a secondary current of 2.4A RMS, NOT primary peaks of 16 Amps. Can anyone help me to understand what is incorrect in my transformer model parameters?

by jaf2009
September 02, 2020

Thanks for the insights, EF82. Very interesting food for thought. We are accustomed to view the world at the macro level, yet in the timing parameters I was asking for the micro level. Curiosity led me to pull some Littelfuse Data sheets on their "Fast Acting" fuses. A 2 Amp fuse could process 18A for .01 sec - longer than those peaks. Hence, at the macro level - No Blow!

Ok, I have a transformer - 230VAC RMS to 12.6VAC RMS - and I am trying to view the circuit from that view. RMS is by definition a mean over time. I am new to simulators, and very much a Bob Pease (Linear Technologies) type - plug in the real components and let them talk! I have used that approach for many successful designs, but now I would like to add simulations to my bag of tricks.

How do I get the simulator to talk to me and present results at more of the macro level?? I think I need to somehow tell the simulator to present RMS type results, no??
I would very much appreciate your efforts in helping me in this learning process.

by jaf2009
September 03, 2020

2 Answers

Answer by jaf2009

This is very helpful, EF82. The Laplace Block opens up a lot of opportunities - I need to spend more time experimenting with it. It certainly looks like this will give me all I need. Many thanks for your time and efforts. John

ACCEPTED +1 vote
by jaf2009
September 04, 2020

Answer by EF82

1] "Stray" DC

Have a close look at the XMFR.nPRI_A current at the start of the T-D simulation plot (0 to 0.016 sec). It goes from 0 to 17.2A and back to 0, that is, a DC current in an AC circuit! Now look at the final cycle of the plot, the PRI current ends at -1.3A. What we see is a time constant in the primary (100mH/0.1Ohm = 1Sec) reducing a DC "kick" from the first half cycle of the input voltage.

Try this experiment:

Add 5sec to both the Start and Stop times of the T-D sim setup. You should find that the PRI current is now +/- 8.6A.

This is one of those occasions (and I've had many) when CL does EXACTLY what you tell it to do, not what you want!!

2] Reactive current

The impedance of 100mH at 60Hz is approx 37 Ohms, so peak (reactive) current is expected at 325/37 = 8.7A (I've ignored PRI resistance). Does this change your view of the size of input fuse a real circuit might need?

I would like to devise demonstrations of all this using the REAL() and IMAG() expressions on circuit currents, but they work only in the Frequency domain. Nevertheless, hoping that there is enough here to help you move on to more investigations.

+1 vote
by EF82
September 03, 2020

Practical update to earlier theoretically-based observations.

Finding even an approximate value for the inductance of a transformer primary is a tricky business. In more technical terms, there are many variables related to flux level, hysteresis in the laminationed-iron core, and frequency: basically, it's non-linear. I've been able to retrieve the details of some "measurements" I made earlier in the year on two small transformers (no spec available for either).

a) Small, low VA 240v mains to 6v: pri around 5H, resistance 1kOhm;

b) Tiny audio output: pri 0.7H, resistance 75 Ohm.

Looking at the Tamura spec it looks a higher VA than (a) so likely lower inductance and resistance. Perhaps 2H and 100 Ohm - just a guess, though.

If you are a keen experimenter, I highly reccommend that you give practical measurement a go - given the dearth of useful data to feed a simulator. It will also show you, in a very direct way, the variability in wound components. But also give you valuable practical knowledge. For my very basic "measurements" I used a browser based Audio Signal Generator and the headphone output on an aging PC. There are online videos on this with lots more practical tips.

by EF82
September 03, 2020

Was drafting a response to your first comments while you were sending the second. I have good empirical data for these Tamura transformers (6-30VA) and have used them a good bit. However, the model has limited inputs available. Moreover, I think I am asking for results at a different level as discussed previously.

by jaf2009
September 03, 2020

Many thanks for further information about what you are doing; good to hear about a solid practical approach.

I have arranged a neat circuit idea from @mrobbins for using controlled voltage sources and "1/s" Laplace blocks as integrators. Perhaps these sorts of outputs might meet some of your macro view criteria.

by EF82
September 04, 2020

Your Answer

You must log in or create an account (free!) to answer a question.

Log in Create an account

Go Ad-Free. Activate your CircuitLab membership. No more ads. Save unlimited circuits. Run unlimited simulations.

Search Questions & Answers

Ask a Question

Anyone can ask a question.

Did you already search (see above) to see if a similar question has already been answered? If you can't find the answer, you may ask a question.

About This Site

CircuitLab's Q&A site is a FREE questions and answers forum for electronics and electrical engineering students, hobbyists, and professionals.

We encourage you to use our built-in schematic & simulation software to add more detail to your questions and answers.

Acceptable Questions:

  • Concept or theory questions
  • Practical engineering questions
  • “Homework” questions
  • Software/hardware intersection
  • Best practices
  • Design choices & component selection
  • Troubleshooting

Unacceptable Questions:

  • Non-English language content
  • Non-question discussion
  • Non-electronics questions
  • Vendor-specific topics
  • Pure software questions
  • CircuitLab software support

Please respect that there are both seasoned experts and total newbies here: please be nice, be constructive, and be specific!

About CircuitLab

CircuitLab is an in-browser schematic capture and circuit simulation software tool to help you rapidly design and analyze analog and digital electronics systems.