Modeling I-V Characteristics in LTSpice

In summary, the conversation discusses how to model the I-V characteristics of diodes in LTSpice and how to display both the forward and reverse breakdown voltage characteristics. It is recommended to use a Zener diode for reverse breakdown and to edit the description of the diode in the program files for more accurate simulations.
  • #1
crono1009
15
0
I'm trying to model the I-V characteristics of a few diodes in LTSpice. Though doing the DC sweep I have in the picture doesn't seem to give me what I want. I'm sweeping from -80V (It's breakdown is 75V) to 2V, in 1V increments.

What kind of simulation do I have to run across the diode to get a nice curve representing the I-V characteristics of a diode?

Thanks!
 

Attachments

  • Diode IV.jpg
    Diode IV.jpg
    12.6 KB · Views: 4,556
Engineering news on Phys.org
  • #2
Make the resistor 0.1 ohms. Vary the voltage from 0 to +2 volts in steps of 0.01 volts.
View the current in the diode.

Run the simulation then left click on the vertical axis and set the maximum current to 100 mA with 10 mA ticks.

This gives a fairly good version of the forward characteristic.
 
Last edited:
  • #3
Thanks for the tips. I am happy with my cut-in voltage, around 0.7V where it should be.

Though I'm having another dilemma, I want to display my breakdown voltage characteristics also. The breakdown voltage of my 1N4148 diode is 75V. So I swept my DC voltage source from -100V to +2V in 0.01V increments, though as you can see from my graph my diode does not conduct in reverse bias at all.

Any thoughts?
 

Attachments

  • Diode IV.PNG
    Diode IV.PNG
    9.6 KB · Views: 3,304
  • #4
LTSpice does not seem to use maximum ratings although they are listed in the diode characteristics. I couldn't see anywhere to turn this on.

I started a trace at -1000 volts and a 75 V diode did not conduct until it was forward biased. It was also able to conduct hundreds of amps where this was unlikely in practice.

If you want a reverse breakdown, try using a Zener diode. LTSpice has quite a few of them.

Use very small steps like 0.01 volts and remove the 1 K resistor because that affects the shape.
 
  • #5
I had a play with this.

Go to
c:\Program Files\LTC\LTspiceIV\lib\cmp\standard.dio
and in the description for the 1N914 edit the text to add "bv=75" after Cjo

Restart LTSpice and reload the simulation.

The simulation now includes a breakdown at -75 volts.
 

1. What is LTSpice and how is it used in modeling I-V characteristics?

LTSpice is a free circuit simulation software that is commonly used in electronics and electrical engineering. It allows users to model and simulate the behavior of electronic circuits, including the I-V characteristics of different components. It uses a graphical user interface to input circuit elements and simulate their response to various inputs.

2. How do I model I-V characteristics in LTSpice?

To model I-V characteristics in LTSpice, you need to first define the circuit components and their parameters. This can be done by selecting the appropriate components from the LTSpice library or by creating custom models. You can then add voltage or current sources to the circuit and simulate their behavior to obtain the I-V characteristics.

3. What types of components can be modeled in LTSpice for I-V characteristics?

LTSpice allows users to model different types of electronic components such as resistors, capacitors, inductors, diodes, transistors, and operational amplifiers. It also has a library of commonly used models for these components, making it easier for users to simulate their behavior.

4. Can I simulate non-linear I-V characteristics in LTSpice?

Yes, LTSpice allows users to simulate non-linear I-V characteristics by using non-linear component models such as diodes and transistors. These models take into account the non-linear behavior of the component and provide a more accurate simulation of the I-V characteristics.

5. How accurate are the I-V characteristic simulations in LTSpice?

The accuracy of I-V characteristic simulations in LTSpice depends on the accuracy of the component models used and the simulation settings. LTSpice provides a variety of models for different components, and users can also create custom models for more accuracy. It is important to carefully select and calibrate the models to obtain accurate simulations.

Similar threads

Gain limiter circuit in LTspice - current flowing in wrong direction
    • Electrical Engineering
Replies
7
Views
1K
ABC reference frame synchronous generator modelling in Ltspice
    • Electrical Engineering
Replies
1
Views
950
Trouble building a Buck Converter
    • Electrical Engineering
Replies
14
Views
807
Building a Buck Converter Using the LT1170
    • Electrical Engineering
Replies
10
Views
1K
Line filter, proper LTspice simulation
    • Electrical Engineering
Replies
15
Views
4K
Voltage offset differential amplifier
    • Electrical Engineering
Replies
11
Views
2K
How Can I Identify a Metal Diode with Specific Voltage Requirements?
    • Electrical Engineering
Replies
7
Views
1K
I-V characteristics of a diode
    • Electrical Engineering
Replies
3
Views
1K
Engineering Understanding the output waveform and using LTSpice
    • Engineering and Comp Sci Homework Help
Replies
1
Views
1K
Solving 555 Based Switcher Challenge for Niхie Clock
    • Electrical Engineering
2
Replies
44
Views
4K

Hot Threads

Recent Insights

Back
Top