Tonefiend Forum

Welcome Guest 

Show/Hide Header

Welcome Guest, posting in this forum requires registration.

Pages: [1]
Author Topic: LTSPICE - The Varitone Zone

Posts: 192
Post LTSPICE - The Varitone Zone
on: August 15, 2012, 11:19

All right, let's start with the Varitone schematic:


Now let's see how I have entered this into LTSpice:


I am using the .step simulation command to step the capacitor through the listed values. The 10 Meg resistors are there to bleed off DC from the caps to eliminate pops when switching and so I left them out from my schematic. If you put them in you'd see little difference in the results. I am also driving this with just a straight voltage source rather than one of my pickup models, because I want to focus on the Varitone response in isolation first. I left the 500k volume pot off too! I'm just terrible!

Here's the frequency response for those 5 caps:


Uploaded with

Now let's take a look at the effect that the series resistor R1 has on the shape of the response. In this case I set the value of C1 to 0.22u instead of the variable Cv, and made R1 track the variable Rv instead of being fixed at 100k. The step values are 1k, 10k, and 100k.



Note that the .step simulation command in blue has been "commented out" so it is not active for this next simulation.


Uploaded with

You can see that when the series resistor is 1k (green trace), the width of the notch is very small, while when it's at 100k (red trace) the notch is very wide. If you were to use a pot here, you might decide that the narrowest notch is not a useful setting. By putting a 10k resistor in series with a 100k pot, you could start the knob's effect at the 10k line (blue trace) instead of the 1k line. Circuit simulation (along with your ears) can help you dial in your guitar's wiring for the best range of tones from your controls.


Posts: 192
Post Re: LTSPICE - The Varitone Zone
on: August 15, 2012, 11:29

Here is the above circuit. To create the ASC file that is readable by LTSpice, copy and paste the text between the two lines into Notepad on your PC, then save the file as Varitone.txt. Then change the extension from txt to asc. Now double click on Varitone.asc and it will open up in LTSpice.

To run the simulation, click on the toolbar icon that looks like a little runner.

The first time you do this, the plot will probably be empty. Right-click on the plot and select "Visible Traces". Choose V(output). If you still don't see anything, right-click on the plot and select "Autorange Y-Axis".

You may also wish to adjust the vertical axes (gain in dB is on the left, phase shift in degrees is on the right). Right click on the plot and choose "Manual Limits". Enter the desired endpoints and/or major divisions and press "OK". One annoyance is that these limits are not preserved if you run the simulation again.

To change values, either of a simulation command, or a component, right click on it. I will gladly try to answer any questions either about using LTSpice, or the results of these simulations.

Version 4
SHEET 1 880 680
WIRE 208 64 128 64
WIRE 336 64 288 64
WIRE 480 64 336 64
WIRE 128 112 128 64
WIRE 336 112 336 64
WIRE 336 240 336 192
WIRE 128 336 128 192
WIRE 336 336 336 304
FLAG 128 336 0
FLAG 336 336 0
FLAG 480 64 Output
IOPIN 480 64 Out
SYMBOL voltage 128 96 R0
WINDOW 123 24 124 Left 2
WINDOW 39 0 0 Left 2
SYMATTR Value ""
SYMATTR Value2 AC 1 0
SYMBOL res 304 48 R90
WINDOW 0 0 56 VBottom 2
WINDOW 3 32 56 VTop 2
SYMATTR Value {Rv}
SYMBOL ind 320 96 R0
SYMATTR Value 1.5H
SYMBOL cap 320 240 R0
SYMATTR Value 0.22µ
TEXT -64 -72 Left 2 !.ac oct 20 20 20000
TEXT -64 -40 Left 2 ;.step param Cv LIST .001u .003u .01u .03u .22u
TEXT -64 -8 Left 2 !.step param Rv LIST 1k 10k 100k

Pages: [1]
Mingle Forum by cartpauj
Version: 1.0.34 ; Page loaded in: 0.109 seconds.

Comments are closed.