Archive for the 'Component Technology' Category

Simulating the CD4066 Quad Bilateral Switch With LTspice

Monday, December 12th, 2011


Ron Fredericks writes: Today is Robert Norton Noyce’s birthday (born 12/12/1927) – co-inventor of the integrated circuit (IC). So I thought I would take a few minutes and document my work modeling the CD4066 quad bilateral switch with the LTspice simulator.

In this post I describe how flexible LTspice can be as a general SPICE circuit simulator, and how accurate its behavior can be in comparing LTspice test results with the physical IC’s datasheet. In this example I use the CD4066B as the IC to model. I test the model using its characteristic “on” resistance curves under various voltage and current operating conditions. I conclude by using a standard CD4066 datasheet to verify the accuracy of the model.

Meanwhile this is the last IC I need to simulate the analog section of the digital volume control circuit using LTspice I mentioned in two of my previous blog entries:

Define one of four bilateral switches on CD4066 for LTspice

 

To get the CD4066 IC into my circuit simulation, I first created a symbol for one of the four bilateral switches in this package, and defined a SPICE subcircuit definition for the switch using existing SPICE CD4007 gate models as the starting point.

Symbol for one of four bilateral switches on the CD4066 IC

 

LTspice symbol for one of four bilateral switches on cd4066 (click to enlarge)

LTspice Subcircuit Definition for CD4066
Note the LTspice implementation of the SPICE language is highlighted (below) using my own GeSHi language highlighter library with key sections of the language (.model and .subcircuit) hyper-linked into SPICE language definitions that I have created on the contributor pages of this website. SPICE is a difficult language to highlight using GeSHi because many of the SPICE language constructs are so short that they overlap with longer language constructs. I plan to add more language definitions in the future as my circuit models need them, and I continue to find unique look-up algorithms to match GeSHi language highlighter categories.

 

code=ltspice
  1.  
  2. * CD4066 Analog Switch
  3. * SYM=CD4066
  4. * Transistor models are from LTspice group member kcin_melnick
  5. * See message number 16897, http://tech.groups.yahoo.com/group/LTspice/
  6. * Analog Switch Control In Out Vdd Vss
  7. .SUBCKT CD4066 2 11 4 10 7
  8. X1 2 6 10 7 INVERT
  9. X2 6 1 10 7 INVERT
  10. M1 14 6 7 7 CD4007N
  11. M7 11 6 14 10 CD4007P
  12. M3 11 1 14 14 CD4007N
  13. M4 11 1 4 14 CD4007N
  14. M8 11 6 4 10 CD4007P
  15. .SUBCKT INVERT 1 2 3 4
  16. * Inverter In Out Vcc Vss
  17. M1 2 1 3 3 CD4007P
  18. M2 2 1 4 4 CD4007N
  19. .ENDS
  20. .MODEL CD4007N NMOS (
  21. + LEVEL=1 VTO=1.44 KP=320u L=10u W=30u GAMMA=0 PHI=.6 LAMBDA=10m
  22. + RD=23.2 RS=90.1 IS=16.64p CBD=2.0p CBS=2.0p CGSO=0.1p CGDO=0.1p
  23. + PB=.8 TOX=1200n)
  24.  
  25. .MODEL CD4007P PMOS (
  26. + LEVEL=1 VTO=-1.2 KP=110u L=10U W=60U GAMMA=0 PHI=.6 LAMBDA=40m
  27. + RD=21.2 RS=62.2 IS=16.64P CBD=4.0P CBS=4.0P CGSO=0.2P CGDO=0.2P
  28. + PB=.8 TOX=1200N)
  29. .ENDS

Testing the CD4066 Circuit in LTspice

Finally, I dragged the symbol with subcircuit models into my LTspice program and ran a series of tests to demonstrate the “on” resistance characteristics associated with the switch at various voltage and current values. Note the multicolored graph showing the resistance curves at various VI levels.

 

VI curves and circuit schematic for cd4066 bilateral switch under test (click to enlarge)

Get these files from LTspice Yahoo Group

The 4 main files used to create this demo circuit can be obtained from LTspice Yahoo Group. Special thanks to Helmut Sennewald

See the figure below…

LTspice Yahoo Group File List (click to enlarge)

Comparison of LTspice circuit simulation with datasheet

The TI datasheet compares favorably with my simulations. The LTspice “on” resistance curves and values are nearly exactly the same as those shown in figures 2,3, and 4 of TI’s datasheet (page 6) for the range I tested.

At this stage of development in simulating the analog path for my automatic volume control circuit, I see that the “on” resistance curve may create an unstable signal path under normal audio conditions unless the operating voltage (Vcc ) is much higher than the original circuit’s proposed 5 VDC power supply.

References

Linear Technologies LTspice Landing Page

Texas Instruments datasheet for the CD4066B

What’s All This CD4007 Stuff, Anyhow?
Bob Pease | ED Online ID #6073 | April 5, 1999
http://electronicdesign.com/Articles/ArticleID/6073/6073.html

Fault in CD4066 Model
kcin_melnick | LTspice Yahoo Tech Group Message #16897 | June 24, 2007
http://tech.groups.yahoo.com/group/LTspice/message/16897

Technorati Claim Tag
SH66YHJAPDBA

Technorati Tags: , , , , ,

Introduction to Google Android

Friday, February 5th, 2010


Ron Fredericks writes: Are you new to the google android smartphone platform and developer ecosystem? If so, then this online video produced from LectureMaker‘s high-tech video studio can help you get up to speed very quickly. The video includes several navigation dots along the time line so you can jump to the content you want to watch (once it has downloaded). Expect to get an overview, some sample code demos, and an understanding of the business case behind developing apps for Android from watching this great video presented by Marko Gargenta of Marakana.

Enjoy…

Android Introduction by Marko Gargenta, marakana
Presented by Peter Lam, Mobile SIG Co-chair, Software Developer Forum

Video Link

Technorati Tags: , , , , , ,

Introducing 74HC193 Simulation to LTspice

Monday, April 21st, 2008

Ron Fredericks writes: I have completed the design and test of a new component for LTspice/SwitcherCAD III circuit simulation and schematic capture. In a previous post I discussed my interest in the 74193 presettable synchronous 4-bit binary up/down counter IC for a digital volume control circuit I am building. The circuit simulation described below focuses on how to simulate the 74HC193 IC, but timing and voltage parameters built into this design allow a designer to easily simulate other variants of this IC from high speed Si-gate CMOS HC and HCT devices to low power Schottky TTL devices.

All circuits related to this 74HC193 simulation are available here>

The 74HC193 Component

See figure 1 below for a screen shot of the completed design. The circuit was built from the digital gates in the component library supplied with the original Linear Technology‘s free LTspice tool.

74HC193 Circuit and Related Components
Figure 1 – 74HC193 Circuit and Related Components
View larger image>

To keep the design looking like the original data sheet logic diagram, as published by companies that include NXP Semiconductors and Texas Instruments, a custom “T notS-R FlipFlop” subcomponent and corresponding assembly file was first created. This subcomponent was reused 4 times in the main IC logic diagram. An assembly file called 74hc193.asy was also created. It includes all pins used on the commercial IC except ground and Vcc. The IC’s internal power supply is not simulated by the Linear Technologies’ gates, and so they are not used or required in this design either.

Each gate within the design has a few variables assigned to them so that the IC remains flexible and easy to reuse in new projects:

  • tdgate right td (propagation time delay assigned to each gate)
  • tdgate2 right td (propagation time delay assigned to the D FlipFlop)
  • tripdtgate right tripdt (td’s accuracy band assigned to each gate including the D FlipFlop)
  • vhighgate right logical high value for each gate and D FlipFlop
  • vlowgate right logical low value for each gate and D FlipFlop

These variables can be assigned their corresponding time and voltage values using a .param statement placed in the main circuit. These values are then within scope for automatic reuse by the 74HC193 component and flipflop subcomponent simulations. Below is an example of how parameter assignment can be made (as used in the test circuit described next):

.param tdgate=10n tdgate2=3*tdgate tripdtgate=1n vhighgate=5v vlowgate=0v

(more…)

Technorati Tags: , , , , , , , , , , , , , , ,

Technorati Tags: , , ,

New Gate Design Using LTspice/SwitcherCAD III

Tuesday, April 15th, 2008


Ron Fredericks writes: recently I discovered that I was going to have to create my own IC component and symbol for my on-going digital volume control circuit simulation. My first step was to check in with the LTspice forum on yahoo groups. On the forum I requested any previous design for the IC I needed. I also asked the group’s readership if they thought it was correct to build a new IC from existing low level digital gates – gates that are already supplied with the LTspice distribution by Linear Technologies.

Well, I did not find a previous inventor for my IC simulation, but I did get confirmation that the gate build-up was a common strategy. And, this same forum engineer supplied me with a copy of an IC simulation of his own – one very similar to my IC requirement – he supplied a symbol and sample test bed to accelerate my learning curve. Here is a link to my support dialog.

I would like to thank Helmut Sennewald for his time and excellent service to the LTspice yahoo forum. It is his effort and many others who make this forum such a valuable community resource. This forum in turn, has made the LTspice/SwitcherCAD III circuit capture and spice tool a viable design tool for many embedded component users and EE designers.

Introducing the T S-R Flip-Flop

To build my new IC, I had to build a new digital logic block. This component is a Toggle Flip-Flop with Set and Reset functions added. In this blog post I introduce my readers to this new component and share the simulation circuit for others to use and learn from.

See the figure below for an initial design of the T S-R Flip-Flop, including a truth table in the form of a waveform diagram, the circuit, a pulse detector sub-circuit and their related assemblies. This circuit is just an initial design because it uses an S-R Flip-Flop and a simple pulse detector sub-circuit for its clock.

T S-R Flip-Flop and releated sub-circuits and assemblies

View larger image>

Final Design for the T S-R Flip-Flop

This section of my post is an update, thanks to a review by Helmut Sennewald. See figure below for my final design of the Toggle S-R Flip-Flop. This design overcomes two problems in my initial design, both resolved by starting with the D Flip-Flop with its built-in clock. The reuse of this more full-featured LT supplied component in my design eliminated the home-brew pulse maker sub-circuit. And in so doing, the slower S-R Flip-Flop. Slower because I had to set the SpiceLine time delay to a minimum of 20 nanoseconds (or td >= 2x the gate time delay) to support the simulation of my simple pulse maker sub-circuit. The D Flip-Flop has an internal clock so I could eliminate the pulse maker sub-circuit. End result: one less sub-circuit and faster Flip-Flop simulation using a time delay set to a minimum of 10 nanoseconds (or td >= 1x the gate time delay).

T S-R Flip-Flop (final design)

View larger image>

Download

To test my knowledge of digital design using the LTspice tool, I created a number of similar flip-flop components which are included in the download:

  1. S-R Flip-Flop test circuit
  2. S-R Flip-Flop with Enable gate and test circuit
  3. S-R Flip-Flop with rising edge clock and test circuit
  4. J-K Flip-Flop with rising edge clock and test circuit
  5. D Flip-Flop with Enable gate and test circuit
  6. T S-R Flip-Flop from S-R Flip-Flop and test circuit (initial design)
  7. Rising Edge Pulse Detector (not high performance design)
  8. T S-R Flip-Flop from D Flip-Flop and test circuit (final design)

Download the components listed above for your LTspice designs all in one zipped directory.

Technorati Tags: , , , , , , ,

Simulating the 555 IC with LTspice

Wednesday, March 26th, 2008


Ron Fredericks writes: I was designing a simple CMOS timer circuit around a 555 chip this evening. It might be the heart beat for a new digital volume control I have been thinking about. Normally I look for my breadboard and parts box but this time I thought I would try out Linear Technologies LTspice/SwitcherCAD III workbench instead.

SwCAD III First Time Use

The tool is free and comes with a lot of support. I downloaded the software and installed it very easily on my Windows XP PC. It includes a graphical schematic design tool with lots of ready made simulated components, including an NE555 for my initial project. Designing the circuit with the built-in CAD tool works very intuitively. While the LTspice simulation took a bit of head scratching before it worked for me.

I was able to configure and run the simulation using the drop down tools menu and the little “running person” icon on the tool bar. But all I could get out of the simulation was a black screen with voltage and timing ticks along the left and bottom edges. So my first problem was in realizing that the visual display would remain black and traceless until I put the mouse cursor over a wire then click. When the little instrument probe showed up as my mouse icon, I realized what was going on here. With the mouse click, waveform tracings would appear in the black panel.

My second problem was that the circuit would not oscillate. Not good for an oscillator design. First, I forgot to connect the 555′s threshold + trigger pins to the R2-C2 node using the wire tool. But still no oscillation, just flat line traces were observed. Now I already know that getting circuits to oscillate follows Murphy’s Laws: Oscillators remain stable, Amplifies and Buffers oscillate, whenever possible. I found a note on the Old School Hacker blog with a fine solution. You must simulate the circuit with a power supply starting from 0 volts rather than just have an instant on Vcc power supply.

In hind sight dah, its the initial transient response from the circuit’s components that kicks the oscillator into oscillating.

After a little practice I improved the schematic diagram with the use of named nodes and seperation of the temporary load resistors R3 and R load from the more permanent circuit components. The load resistors are just place holders for a real load to be added to the circuit schematic next. Look for my next blog post on this subject.

Finally, I used the cursor measurement facility built into the LTspice window (trace window). With this feature, I was able to make “real” measurements on the waveform for frequency and duty cycle.

Circuit

Here is what I was able to generate using the LTspice/SwitcherCAD III tool:

LTspice/SwitcherCAD III circuit diagram and waveforms

View larger image>
Download 555 Astable Flip-Flop Schematic Circuit Diagram>

Referring to the figure above:
   Green Trace -> Output (IC 555 pin 3)
   Blue Trace -> Trigger / Threshold (IC 555 pins 2 & 6)
   Red Trace -> Discharge (IC 555 pin 7)

The Astable Multivibrator

The circuit shown above will trigger itself and free run as a multivibrator. The capacitor C2 charges through resistors R1 and R2 yet discharges through R2 only. Thus, the duty cycle (D) may be precisely set by the ratio of these two resistors. The capacitor charges and discharges between 1/3 Vcc and 2/3 Vcc. But the initial pulse charges C2 starting from 0 Vcc and so this first pulse duty cycle is unique. Since the charge rate and the threshold levels are directly proportional to the supply voltage Vcc, the frequency of oscillation (f) is independent of the supply voltage.

Frequency Calculation Duty Cycle Calculation
   
f = 1.38/{(R_1 + 2R_2)C_2} D = {tau}/T = {R_1 + R_2}/{R_1 + 2R_2}
   
1.7 hertz=1.38*10^3/{(150 + 2*332) ohm farads} 0.59~={150 + 332}/{150 + 2*332}
   
Measured = 1.8 hertz Measured = 0.60
   
Where:
    f is frequency in hertz
    C is capacitance in farads
    R is resistance in ohms
Where:
    D is duty cycle
    tau is non-zero output duration
    T is the period of the output
    R is resistance
   

Reference

Technorati Tags: , , , , , ,

How to Leverage the Value of a Board Support Package

Wednesday, November 21st, 2007


Ron Fredericks writes: There are three separate views to what defines an effective Board Support Package (BSP). I believe each of these views is correct as independent descriptions of a BSP. But together these views provide insight into the embedded target from equally important perspectives or engineering disciplines. Read this post to learn more about the essence of embedded systems and how Wind River’s VxWorks BSP architecture has been a critical success factor in comparison to many other real-time embedded operating system executives and kernels available today.

I chose to discuss Wind River’s VxWorks BSP because of my familiarity with their product line, my understanding of their BSP as a competitive product compared to other real-time kernels, and because of my industry accomplishments working with Wind River’s BSPs:

  • Ron Fredericks wins Wind River’s prestigious Navigation Award for designing, launching, and marketing the first online interactive social network for BSP’s. more>
  • Ron Fredericks wins Aiysis’ Million Dollar Club Award for nurturing a Wind River partnership between VxWorks and Aiysis DriveWay BSP tool kit that generated over one million in annual sales. more>
  • Ron Fredericks co-author’s an article with Xilinx on How to Design Field Upgradable Systems based on FPGA Internet connectivity with VxWorks BSP’s. more>
  • Ron Fredericks produces an online video: How to Prototype a Device Driver [or BSP] in Less Than – Wow! – 5 Minutes for a Freescale application processor / communications co-processor System on Chip (SoC). more>

A similar high level discussion can not be made for most embedded Windows or embedded Linux BSP’s today. This is because the BSP for these monolithic kernels are not as modular as a real-time executive kernel such as VxWorks. Indeed other real-time kernel vendors can and do take advantage of the BSP too. But, the VxWorks BSP just took more advantage of this natural separation between board support and kernel tasks earlier in the marketplace and has been an advantage for its customers as a result ever since.

Target Board with BSP connected to a host workstation
Figure 1 – Embedded device with BSP connected to a host workstation

As shown in Figure 1, most BSP’s today, even those for embedded Windows and embedded Linux, do have a robust set of boot options. In many cases a BSP can be used on its own to network attach to a shared file system where the full operating system and application can be loaded. In this way, a device under development need not be the device where development takes place. The BSP in this case forms the basis for a cross-platform development environment – a big plus for developers of embedded systems. Developers often expect cross-platform development to include a BSP with a limited network stack to load new code onto the target hardware during a cold reset. The BSP might use JTAG on-chip run-time control, RS232 serial port, FTP, Bootp, TFTP and RARP, or even a command shell with a full network stack, as the boot loading protocol. But what ever host to target connectivity is used, cross-development allows a high end workstation to be used for time-saving development along with an easy way to download the resulting compiled relocatable object code or a linked and located image onto an embedded target.

For hardware vendors, the BSP is a very useful partner tool. If a hardware vendor makes a set of boards along with a bus pre-assembled as a subsystem or just a single board computer, the BSP allows its clients to leverage this hardware for software development right away. So a hardware vendor can select major operating systems that meet the needs of its target client base and offer a BSP suitable for these operating systems. Usually the BSP is not a licensed product from the operating system vendor and can be bundled royalty free or under very libral license fee conditions. In this way, the operating system vendor or the open-source community, can partner with this hardware platform as a known reference for direct end products or for development of custom products. The horrible alternative is a slow hardware bring-up using new hardware for the first time to build a unique BSP – a very slow and expensive procedure where few software debug tools are available. JTAG or other N-wire run-control devices can be used with an operating system vendor’s debugger in some cases when a robust BSP is not already available. Silicon vendors and I/O device vendors can leverage this technical marketing strategy too.

I encourage Microsoft and embedded Linux communities to consider improving their BSP strategy to deliver more value from a separate BSP structure too. I also encourage my readers to go ahead and submit comments to this blog post if you know of other vendors with good BSP designs as the marketplace is always changing.

(more…)

How to build Dean Lee’s Syntax Highlighter from latest components

Tuesday, May 29th, 2007

Ron Fredericks writes: In my last two posts:

During my research to solve the word wrap problem, I discovered a few more issues leading me to update Dean’s plugin with the latest version of GeSHI (an open-source project: Generic Syntax Highlighter for php. Highlight many languages, including PHP, CSS, HTML, SQL, Java, Assembler, and C for XHTML compliant output) and removal of unused files. I thought other WordPress bloggers might like to take advantage of the latest code too, so I document the steps needed to build a clean plugin with the latest components.

Flow Chart / Swim Lanes Widget
Below is a Flash widget I built to document the steps needed so you can roll your own up-to-date plugin. Follow these steps and you won’t have to be a programmer to get the benefits from the latest versions of these program components. The widget actively links to the latest PHP files and CSS classes:

(more…)

Technorati Tags: , , , , , , , , , , ,

Online Lecture: Common Internet File System

Wednesday, December 6th, 2006

CIFS Embedded Device Block Diagram
Ron Fredericks writes: Recently I came across a reference to an article I wrote for ISA, sponsored by Visuality Systems, on Brian Mork‘s Increa Technology Blog. The article presented the emerging use of the Common Internet File System (CIFS) for connecting industrial instruments from the plant floor to the engineering work stations and on into business operations.

Embedded Components, Inc. has a short [and free] online lecture introducing the CIFS protocol to the embedded device manufacturing community. The CIFS protocol is likely the most ubiquitous file sharing middleware used in the desktop and enterprise computer markets today. Wow! If its so common why haven’t I seen it? Its embedded so it just works in the background.

What is the CIFS standard?

What is the new event presented in this online lecture?

  • CIFS NQ is available for {many embedded and real-time operating systems such as VxWorks, Integrity, and threadX} now
  • Prior to CIFS NQ, there was no practical way for an embedded designer to take advantage of this very easy to use and very common desktop computer protocol

References:

Technorati Tags: , , , , , , , , , , , , , , , , , , , , ,