# Creating a voltage clipper/limiter circuit with only one AC source?

I'm trying to create a clipper circuit that clips the voltage on a load to something between -6 V and 7 V.

If I apply a source with a changing voltage (AC increasing from -10V to 10V for example with increments of 0.1 V) the load can have that source's voltage as long as it's between -6 V and 7 V but if it's under -6 V it'll be clipped to -6 V and if it's above 7 V it'll be clipped to 7 V.

I know how to design this circuit using additional sources/batteries but I'm trying to design it using only one source along with resistors and diodes only.

Any suggestions? I tried a few methods but I couldn't design the circuit. Will a Zener diode do the trick?

I'm trying to implement and simulate this in LTSPICE.

Your input is very valuable and thank you.

• Is a high impedance okay? The simple way is a resistor+zener based circuit Commented Jan 24, 2022 at 3:02
• Look at voltage regulator circuits for inspiration Commented Jan 24, 2022 at 3:03
• @user253751High impedance is okay. How do I possibly implement that? I'm having a difficulty because it's from -6 to 7 (not -6 to 6 for example) Commented Jan 24, 2022 at 4:31
• most voltage regulator circuits seem to have transistors in them and I can't use that. I'll check more of them out hopefully I'll see something that could work. Thank you! @user253751 Commented Jan 24, 2022 at 4:31
• Please clarify your specific problem or provide additional details to highlight exactly what you need. As it's currently written, it's hard to tell exactly what you're asking.
– Community Bot
Commented Jan 24, 2022 at 6:54

You can put two zeners back to back, in each direction the voltage will be the zener voltage of the reverse biased diode plus the forward drop of the forward biased diode.
If you need to get zeners in LTSpice with different voltages you can make a new model using AKO (A Kind Of) to change a parameter of an existing zener model like this:

.model zlowlimit ako:1N750 BV=5.2


You then put your diodes in the circuit, hold Ctrl and right click the diode, and then change the Value to the name of your new model.
This will get it working in LTSpice, in the real world you would need to find diodes with the forward and reverse characteristics to fit your needs.

Edit: I just noticed the requirement for a 1000 ohm load, I used 10,000 but it shows the basic idea, you'd just need to adjust the values.

• No need for two diodes, one is enough: .model d d ron=10m roff=10meg vfwd=6 vrev=7 epsilon=0.1 revepsilon=0.1. Or use a behavioural source with limit(), or with the more convergence-friendly uplim(dnlim()). Or use the [SpecialFunctions]/ota for a tanh() limiting (simple smooth/hard limiting also available). Commented Jan 25, 2022 at 18:12
• I'm going with the idea that someone would eventually want to make this out of actual diodes. Sure you could make up a diode like that, but it doesn't really buy you anything except one less part in the simulation. Commented Jan 25, 2022 at 18:23
• "but it doesn't really buy you anything except one less part in the simulation" -- that is the point. ;-) It will be one element and one node less in the matrix, not to mention less computation because the diode is not just a simple arithmetic operation. It may not matter in the simple example you posted, it may not matter even in a complicated schematic. Nevertheless, it can account for good simulation practice to be efficient. Or not, it's always a choice. Commented Jan 25, 2022 at 19:59