Are you interested in nanotechnology based AI processors?

Sign up for our newsletter for progress updates, product announcements and news.

Knowm Memristor Array

Overview

This is the second in a series of posts that I will be publishing to serve as tutorials for using the Knowm OSS EDA Stack to support the design, layout and simulation of memristors and neuro-memristive circuits and devices. This post will cover three additional memristor models which are available in the Known OSS EDA – Xyce-6.6 release candidate 1. The first model is the TEAM model developed by Shahar Kvatinsky, Eby G. Friedman, Aninoam Kolodny and Uri C. Weiser and presented in a paper titled TEAM: ThrEshold Adaptive Memristor Model, published in IEEE Transactions on Circuits and Systems -I: Regular Papers, Vol. 60, No. 1, January 2013. The second model is the Yakopcic model developed at the University of Dayton, by Chris Yakopcic and presented in a paper titled, Memristor Device Modeling and Circuit Design for Read Out Integrated Circuits, Memory Architectures, and Neuromorphic Systems, published in 2014 as part of the requirements for a PhD in Electrical Engineering. The third model is the Joglekar model developed by Biolek et al., published in 2009 titled, SPICE Model of Memristor with Nonlinear Dopant Drift, which decribes the mathematical model of the prototype memristor device manufactured in 2008 at HP Labs. The first two models, TEAM and Yakopcic models were added to the Xyce OpenModels library by the Xyce Team at Sandia National Labs. The third Joglekar model is now available within the Xyce Electronic Simulator’s OpenModels library thanks to Tim Molter of Knowm, Inc., and is featured in his post Native Memristor Device Developement in Xyce, Creating the Joglekar memristor model in Xyce from scratch

Prerequisites

• Please follow the installation and configuration of your Knowm OSS EDA Environment found in the tutorial titled Simulating the Knowm M-MSS Memristor Model Using Qucs-S with Xyce

NOTE: The current release candidate for the Knowm OSS EDA Stack is available for macOS Sierra 10.12 and Ubuntu 16.04 LTS (Xenial Xerus). This post covers installation on MacOS and Linux but usage only on the macOS platform. The installation process is different, but the use of the software is more or less the same. There is currently support for Xyce (Serial) simulations. The included versions of Qucs-S (0.0.19S) and Xyce 6.6 include libraries for amd64 (intel) 64-bit architectures. Support for other architectures and operating systems are under development and will be released when available.

Launch Qucs-S

1. Click on the Qucs app icon on the Launcher Bar.

Open a Project File

1. Double click the Ymemristor_prj to automatically open the Content tab.
   

   Qucs Project List

   

   Qucs Project Contents

Create the Schematic diagram

1. Select the Components tab in the Main Dock.

2. Open the sources from the drop down combo box.

3. Select the ac Voltage Source and then left click on the schematic to place the symbol.

4. Press the Esc key to exit place mode.

   

   Qucs Component Sources

   

   AC Voltage Source

5. Open the nonlinear components from the drop down combo box.

6. Select the MR Memristor and then left click on the schematic to place the symbol.

7. Press the Esc key to exit place mode.

   

   Non-linear Components Selection

   

   Components MR1 Memristor

8. Open the probes from the drop down combo box.

9. Select the Current Probe and then left click on the schematic to place the symbol.

10. Press the Esc key to exit place mode.

    

    Component Current Probe

    

    AC Voltage Source, MR1 Memristor and Current Probe

Set AC Voltage Source properties

1. Select the f row in the properties table.

2. Change the frequency from 1 GHz to 10 Hz.

3. Select the display in schematic checkbox.

   

   AC Voltage Source Frequency Setting

4. Click Apply to set the frequency value.

5. Click OK to exit the properties dialog.

6. Open the lumped components from the drop down combo box.

7. Select the Resistor US and then left click on the schematic to place the symbol.

   

   Select Component Resistor US from lumped components

8. Press the Esc key to exit place mode.

   

   Schematic with All Components

   SUGGESTION: Try to place each component’s nodes on the grid. You can either manually position the component using you mouse or right click on the component symbol and select Set on Grid.

Clean up component and set MR Memristor parameters

1. Click on the Resistor symbol and select the Rotate

   

   Toolbar Rotate Button

   button on the toolbar or press Command⌘+R keys to orient the resistor symbol with its text to the right.

2. Right click on the MR1 Memristor symbol and select the Rotate or press the Command⌘+R three times to orient the memristor with the minus terminal in the down position.

   

   Schematic with R1 and MR1 Rotated

3. Right click again on the MR1 Memristor symbol Move Component Text from the context menu.

4. Left click on the MR1 MEMERISTOR label and drag it to a position to the right of the memristor symbol.

   

   MR1 Component with Repositioned Text

5. Left click anywhere on the schematic to exit move mode.

Edit the Value of Resistor R1

1. Right click on the R1 Resistor symbol and select the Edit Properties.

   

   Select R1 to Edit the Properties

2. Select the R row and enter 75 Ohms

   

   Set R1 Resistance Value

3. Click Apply to set the frequency value.

4. Click OK to exit the properties dialog.

Place the Ground nodes

1. Select the Gnd symbol on the toolbar.

   

   Gnd Toolbar Button

   Then left click on the lower terminal of the R1 Resistor to place the symbol on the schematic.

2. Click on the minus terminal of the ac Voltage Source to place another Gnd symbol on the schematic.

3. Press the Esc key to exit place mode.

   

   Schematic with Gnd Nodes Added

Wire the Schematic Components

1. Select the Wire tool button on the toolbar.

   

   Wire Toolbar Button

2. Select the upper terminal of R1 node and then left click the negative node of the MR1 memristor symbol.

3. Press the Esc key to exit place mode.

4. Select the positive node of the ac Voltage Source and then left click the input node of the Current Probe.

5. Select the positive node of the MR1 Memristor and drag to the out node of the Current Probe Pr1.

   

   Schematic with All Components Wired

Add a Named Node (Vmr)

1. Click the Name button on the toolbar.

   

   Named Node Toolbar Button

2. Left click on the positive node of the MR1 Memristor symbol.

3. Enter the Vmr for the label.

   

   Vmr Named Node

4. Click OK to save the changes.

5. Press the Esc key to exit place mode.

6. Click on the Vmr label and drag it to a position below the memristor symbol.

7. Left click on the schematic to exit move mode.

   

   Named Node (Vmr) Set to Retrun Memristor Voltage

Add a Named Node (Vout)

1. Click the Name button on the toolbar.

   

   Named Node Toolbar Button

2. Left click on the connection between R1 and the negative node of the MR1 Memristor symbol.

3. Enter the Vout for the label.

   

   Add Named Node (Vout)

4. Click OK to save the changes.

5. Press the Esc key to exit place mode.

6. Click on the Vout label and drag it to a position below the memristor symbol.

7. Left click on the schematic to exit move mode.

   

   Named Node (Vout) Set to Return Volts Output

Select .Model Directive for the MR1 Memristor Component

The MR Memeristor model is accompanied by several model directives that can be independently applied to each memristor symbol instance in the schematic diagram. These are selected from the Libraries tab. The MR Memristor component is used for multiple model definitions in Xyce. These are selected by the level parameter of the model. The following levels are available for the MR Memristor model in Xyce.

The parameters sets are stored in the .Model card format for SPICE compatible simulators.

• level=2 : TEAM memristor model
• level=3 : Yakopcic memristor model
• level=4 : Joglekar memristor model
• level=5 : Knowm M-MSS memristor model

Xyce Memristor Technology Lib

NOTE: There are 4 different levels for the Memristor Model in Xyce. Each of these correspond to the model parameter sets above. At this point of this tutorial you can select form any of the available models in the Xyce Memristor Technology Library. The selection .Model and assignment to the MR1 Memristor component in the schematic determines the the model being simulated. There are a few other differences in the circuit design based on the model selected. I will point out the subtle changes to the circuit schematic and explain their significance as we proceed through the rest of this tutorial.

To Select the TEAM Model

1. Select the Libraries tab from the Main Dock.

2. Left click on the Xyce_Memristor_Technology to expand the list.

3. Select the appropriate MRM(X) file for the model you want to use. In this case MRM2

   

   MRM2 for TEAM Model

4. Left click to place the .Model directive on the schematic.

   

   Schematic with TEAM Model

5. Press the Esc key to exit place mode.

Assign the MRM2 TEAM Model to MR1 Memristor

1. Double click on the MR1 symbol to open the setup parameters dialog.

2. Select MEMRISTOR line 1.

3. Enter MRM2 for the TEAM model to assign it to the MR1 Memristor compnent

   

   MR1 Component Set MRM2 to use TEAM Model

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

   

   Schematic with MRM2 TEAM Model

Configure the Transient Simulation

1. Select the Components tab from the Main Dock.

2. Open the simulations from the drop down combo box.

3. Click and drag the Transient Simulation and drop it on the schematic and left click to place the symbol.

4. Press the Esc key to exit place mode.

   

   Select Transient simulation

   

   Schematic with Transient Simulation

5. Double click on the transient simulation symbol to open the setup parameters dialog.

   

   Transient Simulation Settings

6. Enter 1 ns in the Start param field.

7. Enter 1 s in the Stop param field.

8. Enter 101 in the Number value field to set a 10 ms step size.

9. Click Apply to save the changes.

10. Click OK to exit the properties dialog.

    

    Schematic with Transient Simulation Parameters Set

Save the Schematic Diagram File

1. Click the Save button on the toolbar.

   

   Save Toolbar Button

2. Enter the filename team_mr_test for the schematic diagram.

3. Click Save to save the schematic to the .sch file.

Run a Simulation

1. Press F2 or select Simulation/Simulate menu item or click the Run button on the toolbar.

   

   Run Simulation Toolbar Button

2. Check simulation for errors or warnings. See the status bar at the bottom of the Qucs window lower right corner.

   

   External Simulation Window

3. Click the Exit button to close the Simulation window.

4. You can view and messages written by the simulator by clicking the F5 key or selecting Show Last Messages from the Simulations menu.

   

   Xyce Message Log

5. You can save the current netlist by clicking the Save Netlist button on the simulation window.

   NOTE: The F6 key or Show Last Netlist from the Simulations menu currently only displays the last netlist for the lastest Qucsator simulation. If you save the netlist using the button on the simulation window then you can open the .cir file under Others list in the project tree.

   

   Qucs-S Generated Netlist

Set Document Settings (Optional)

For smaller sized schematics it is often desirable to add the data tables and plots to the schematic diagram. The default behavior is for the data to displayed in a separate tab after the simulation is complete. You can change this behavior by changing the settings for the schematic diagram.

1. Right click on the schematic and select Document Settings...

2. Select Simulations tab.

3. Uncheck open data display after simulation checkbox in the dialog.

   

   Document Settings

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

Check Tabular Results

1. Select the Components tab from the Main Dock.

2. Open the diagrams from the drop down combo box.

   

   Component Diagram Tabular Data

3. Select the Tabular and then left click on the schematic to place the table.

   

   Tabular Diagram Settings

4. Double click on the tran.I(PR1) row to add it to the graph.

5. Double click on the tran.V(VMR) row to add it to the graph.

6. Click Apply to set the value.

7. Click OK to save the changes.

Schematic with Trasient Tabular Results

1. Press the Esc key to exit place mode.

Create a I-V vs. Time Plot

1. Select the Components tab from the Main Dock.

2. Open the diagrams from the drop down combo box.

3. Select the Cartesian and then left click on the schematic to place the symbol.

   

   Component Diagram Cartesian Plot

4. Double click tran.V(VMR) row to add it to the graph.

   

   I-V vs Time Plot Settings

5. Double click on the tran.I(PR1) row to add it to the graph.

   

   I-V vs Time Plot Settings

6. Select the tran.I(PR1) in the Graph window and then select right Axis from the y-axis: drop-down list.

   

   I-V vs Time Plot Settings – PR1 on Y2 Axis

7. Click Apply to save the changes.

8. Click OK to exit the properties dialog.

9. Press the Esc key to exit place mode.

10. Left click anywhere on the plot window and use the corner grab handles to resize the plot.

    

    I-V vs Time Plot

Create a Hysteresis Plot

1. Select the Components tab from the Main Dock.

2. Open the diagrams from the drop down combo box.

3. Select the Cartesian and then left click on the schematic to place the symbol.

   

   Component Diagram Cartesian Plot

4. Double click on the tran.I(PR1) row to add it to the graph.

   

   Hysteresis I vs V Setting

5. Select the tran.I(PR1) in the Graph window.

6. Select tran.V(VMR) in the Plot Vs. dropbox.

   

   Hysteresis I vs V with Plot vs Set to VMR

7. Click Apply to save the changes.

   Notice that the Graph Input changes to xyce/tran.I(PR1)@tran.V(VMR)

8. Click OK to exit the properties dialog.

9. Press the Esc key to exit place mode.

10. Left click anywhere on the plot window and use the corner grab handles to resize the plot.

    

    Hysteresis I vs V Plot

Whew! Now you should have project for TEAM Model simulation. Be sure to save your project before continuing.

TEAM Model Simulation

Yakopcic Model (Additional Exercise)

Try to create the schematic diagram yakopcic_mr_test.sch on your own. You will need to start from scratch with a new schematic. Use the File/New menu option or click the New toolbar button

New Toolbar Button

When creating your new schematic for the Yakopcic memristor test you can omit the current limiting resistor R1 that was present in the TEAM model test circuit because the Yakopcic model does not require this component in order to perform the transient simulation. This will give you a feel for the model characteristics without the addition of the voltage divider configuration of the TEAM model test circuit.

When you have completed the wired schematic you should have all the components placed and wired. Your schematic should look something like this

Schematic with All Components Wired and Vmr

To Select the Yakopcic Model

1. Select the appropriate MRM(X) file for the model you want to use. In this case MRM3
   

   Select MRM3 for Yakopcic Model

2. Left click to place the .Model directive on the schematic.

   

   Schematic with .Model MRM3 for Yakopcic Model

3. Press the Esc key to exit place mode.

Assign the MRM3 Yakopcic Model to MR1 Memristor

1. Double click on the MR1 symbol to open the setup parameters dialog.

2. Select MEMRISTOR line 1.

3. Enter MRM3 for the Yakopcic model to assign it to the MR1 Memristor compnent

   

   Set MRM3 for Yakopcic Model

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

   

   Schematic with MR1 Assignend MRM3 Yakopcic Model

Configure the Transient Simulation

1. Select the Components tab from the Main Dock.

2. Open the simulations from the drop down combo box.

3. Click and drag the Transient Simulation and drop it on the schematic and left click to place the symbol.

4. Press the Esc key to exit place mode.

   

   Select Transient simulation

   

   Schematic with Transient simulation

5. Double click on the transient simulation symbol to open the setup parameters dialog.

6. Enter 1 ns in the Start param field.

7. Enter 1 s in the Stop param field.

8. Enter 101 in the Number value field to set a 10 ms step size.

   

   Transient Simulation Settings

9. Click Apply to save the changes.

10. Click OK to exit the properties dialog.
    

    

    Schematic with Transient Simulation

Save the Schematic Diagram File

1. Click the Save button on the toolbar.

   

   Save Toolbar Button

2. Enter the filename yakopcic_mr_test for the schematic diagram.

3. Click Save to save the schematic to the .sch file.

Run a Simulation

1. Press F2 or select Simulation/Simulate menu item or click the Run button on the toolbar.

   

   Run Simulation Toolbar Button

2. Check simulation for errors or warnings. See the status bar at the bottom of the Qucs window lower right corner.

   

   External Simulation Window

3. Click the Exit button to close the Simulation window.

Try to reproduce the Tabular and Cartesian Plot setup on your own. You can refer back to the TEAM Memristor section of above if you need a hint. When you have completed this section your schematic should look something like the following image.

Yakopcic Model Simulation

Joglekar Model (Additional Exercise)

Again try to create the schematic diagram joglekar_mr_test.sch on your own.

For this exercise let’s change the AC Sinusoidal amplitude for this model simulation. To change the voltage of the AC sinusoidal voltage source do the following.

Set AC Voltage Source properties

1. Double click on the ac Voltage Source symbol to open the parameters for the source.

2. Select the U row in the properties table.

3. Change the voltage from 1 V to 500 mV.

4. Click Apply to set the voltage value.

   

   AC Voltage Source Settings

Your schematic should now look something like this:

Complete Wired Schematic

To Select the Joglekar Model

1. Double click on the MR1 symbol to open the setup parameters dialog.

2. Select MEMRISTOR line 1.

3. Select the appropriate MRM(X) file for the model you want to use. In this case MRM4

   

   Joglekar model MRM4

Assign the MRM4 Joglekar Model to MR1 Memristor

1. Double click on the MR1 symbol to open the setup parameters dialog.

2. Select MEMRISTOR line 1.

3. Enter MRM4 in the param list and model spec field.

   

   Enter MRM4 for MR1 Memrsitor

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

   

   Joglekar model selected for MR1

Configure the Transient Simulation

1. Select the Components tab from the Main Dock.

2. Open the simulations from the drop down combo box.

3. Click and drag the Transient Simulation and drop it on the schematic and left click to place the symbol.

4. Press the Esc key to exit place mode.

   

   Select Transient simulation

   

   Transient simulation

5. Double click on the transient simulation symbol to open the setup parameters dialog.

6. Enter 1 ns in the Start param field.

7. Enter 1 s in the Stop param field.

8. Enter 101 in the Number value field to set a 10 ms step size.

   

   Transient Simulation Parameters

9. Click Apply to save the changes.

10. Click OK to exit the properties dialog.

    

    Schematic with Transient simulation

Configure the R_init Parameter for the MR Memristor Model

Like the KnowmMemristor M-MSS model which we looked in our very first tutorial you need to add the .PARAM directive to set the initial resistance R_init for the model. This again can be accomplished by do the following steps.

1. Select the Components tab from the Main Dock.

2. Open the SPICE specific sections from the drop down combo box.

3. Click and drag the .PARAM Section and drop it on the schematic and left click to place the symbol.

4. Press the Esc key to exit place mode.

   

   Components SPICE Specific

Schematic with .PARAM

1. Double click on the .PARAM symbol to open the setup parameters dialog.

2. Enter R_init in the param field.

3. Enter 11000 in the value field to set R_init=11000 ohms.

   

   Set R_init to Default Resistance

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

   

   .PARAM R_init set to 11000

Set Document Settings (Optional)

For smaller sized schematics it is often desirable to add the data tables and plots to the schematic diagram. The default behavior is for the data to displayed in a separate tab after the simulation is complete. You can change this behavior by changing the settings for the schematic diagram.

1. Right click on the schematic and select Document Settings...

2. Select Simulations tab.

3. Uncheck open data display after simulation checkbox in the dialog.

   

   Document Settings

4. Click Apply to save the changes.

5. Click OK to exit the properties dialog.

Save the Schematic Diagram File

1. Click the Save button on the toolbar.
   
   

   Save Toolbar Button

2. Enter the filename joglekar_mr_test for the schematic diagram.

3. Click Save to save the schematic to the .sch file.

Run a Simulation

1. Press F2 or select Simulation/Simulate menu item or click the Run button on the toolbar.

   

   Run Simulation Toolbar Button

2. Check simulation for errors or warnings. See the status bar at the bottom of the Qucs window lower right corner.

   

   External Simulation Window

3. Click the Exit button to close the Simulation window.

Try to reproduce the Tabular and Cartesian Plot setup on your own. You can refer back to the TEAM Memristor section of above if you need a hint. When you have completed this section your schematic should look something like the following image.

Transient Simulation of Joglekar Model

Conclusion

That completes this three part tutorial. You should also checkout the documentation and other examples listed in the Qucs 0.0.19 and Qucs-S 0.0.19 documentation available on the web at the following URLs. In my next post we will be exploring more dynamic behavior or the Knowm M-MSS Memristor Model with respect to square-wave pulse response by looking at Bi-directional Incremental Conductance Change and other effects.

• Qucs 0.0.19 Help: https://qucs-help.readthedocs.io/en/0.0.19/subcircuit.html
• Qucs-S 0.0.19 Help: https://qucs-help.readthedocs.io/en/spice4qucs/SPICEComp.html
• Qucs-S Bugtracker: https://github.com/ra3xdh/qucs/issues
• Qucs-S Sub-project Home Webpage: https://ra3xdh.github.io/

Other References

• What is Qucs?
• What can all be installed from Sourceforge?
• Qucs Website: http://qucs.sourceforge.net/
• Main Repository: https://sourceforge,net/p/qucs/git/ci/master/tree/
• Mirror Repository: https://github.com/Qucs/qucs
• Mailing lists: http://sourceforge.net/p/qucs/mailman/
• Forum: http://sourceforge.net/p/qucs/discussion/
• Bug trackers:
  • http://sourceforge.net/p/qucs/_list/tickets
  • http://github.com/Qucs/qucs/issues
• Source code documentation:
  • http://qucs.github.io/qucs-doxygen/qucs/index.html
  • http://qucs.github.io/qucs-doxygen/qucs-core/index.html
• Wiki: https://github.com/Qucs/qucs/wiki

Further Resources

• Knowm Memristors
• The Generalized Metastable Switch Memristor Model
• Simulating the Knowm M-MSS Memristor Model Using Qucs-S with Xyce
• The Problem is Not HP’s Memristor–It’s How They Want To Use It
• The Joglekar Resistance Switch Memristor Model in LTSpice
• Build Xyce from Source for ADMS Verilog-A Model Integration
• The Pershin Voltage Threshold Memristor Model in NGSpice
• memristor-models-4-all Project on Github