• State TI Thinks Resolved
  • Locked Locked
  • Replies 2 replies
  • Answers 1 answer
  • Subscribers 41 subscribers
  • Views 419 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

Request for Spice Model of 74LS189 RAM for SAP-1 Computer Simulation.

MARCOS VINICIUS
Prodigy 10 points

Dear Texas Instruments,

I hope this email finds you well. My name is Marcos Vinícius, and I am a dedicated Industrial Automation student with a passion for computer engineering and simulation. I am reaching out to your esteemed company with a unique request.

Recently, I embarked on an exciting journey in collaboration with my advisor to build an SAP-1 (Simple-As-Possible) computer, a project inspired by the work of A. Malvino. The initial phase of our project involves computer simulation using Spice models, a crucial step in understanding the intricacies of the SAP-1's components.

However, we have encountered a significant challenge in sourcing a Spice model for the TTL 74LS189 RAM, an essential component in our project. Despite thorough searches across various electronics forums on the internet, we have been unable to locate a suitable Spice model for the 74LS189 RAM. Hence, I am reaching out to your company in the hope that you might have the expertise and resources to assist us.

My questions are as follows:

  1. Is it possible to obtain a Spice model for the 74LS189 RAM from your company?
  2. Does your organization already possess Spice models for components such as the 74LS189?
  3. Can we effectively simulate the 74LS189 RAM within OrCAD, or are there any specific considerations we should be aware of?

If the answer to my queries is negative, I would appreciate any insights you can provide regarding the absence of a Spice model for the 74LS189. Additionally, I am curious to understand the challenges or complexities involved in creating a Spice model for this particular component.

I am sincerely grateful for your time and consideration of this request. Your assistance would significantly contribute to our educational journey and the successful completion of our SAP-1 computer project.

Thank you in advance for your support. I look forward to your response and any guidance you can provide.

Warm regards,

Marcos Vinícius de Freitas
marcos.vf@

  • 0
    TI__Guru 71526 points

    Hello Marcos, 

    The SN74LS189 is a very old device, not in our portfolio for decades.  I will continue to enquire, but I doubt there will be any information pertaining to this device.  

    Regards,

    ~Leonard  

  • 0
    TI__Guru* 96712 points

    Hi Marcos,

    We don't have models on hand for this device, or really any of the older bipolar logic like this device. On top of being from an old logic family, this is also a latched logic device, which has additional problems for creating a model. I've found that SPICE doesn't really do so well with latching logic circuits like memory - they tend to produce singular matrices in the nodal analysis.

    Modern simulators get around this by using integrated digital back-ends, and those are unique to the specific simulator. If you dig around in PSpice, you can find libraries for the 74LS logic family that have a fairly good set of devices supported -- on my computer, this is located in C:\Cadence\SPB_17.4\tools\pspice\library\74ls.lib

    Here's an example model from the library for the D-type flip-flop:

    *---------
* 74LS74  Dual D-Type Positive-Edge-Triggered Flip-Flops w/ Preset & Clear
*
* The TTL Data Book, Vol 2, 1985, TI
* tdn	06/28/89	Update interface and model names
*
.subckt 74LS74A  1CLRBAR 1D 1CLK 1PREBAR 1Q 1QBAR
+	optional: DPWR=$G_DPWR DGND=$G_DGND
+	params: MNTYMXDLY=0 IO_LEVEL=0
UFF1 dff(1) DPWR DGND
+	1PREBAR 1CLRBAR 1CLK   1D   1Q 1QBAR 
+	D_LS74 IO_LS MNTYMXDLY={MNTYMXDLY} IO_LEVEL={IO_LEVEL} 
.ends
*
.model D_LS74 ueff (
+	twpclmn=25ns	twclkhmn=25ns
+	tsudclkmn=20ns	thdclkmn=5ns
+	tppcqlhmx=25ns	tppcqlhty=13ns
+	tppcqhlmx=40ns	tppcqhlty=25ns
+	tpclkqlhty=13ns	tpclkqlhmx=25ns
+	tpclkqhlty=25ns	tpclkqhlmx=40ns
+	)
*$

    The important thing to note here is the compoent type in the model -- the "UFF1" is a PSpice-specific model. It won't work in any other simulator.

    You could, in theory, utilize their digital back-end to write your own LS family RAM model to support the LS189 function. The input/output structures are shown in the datasheet, so you can use those directly to give a fairly good analog simulation of the I/O characteristics, then connect them to a model of your own design for housing the digital memory blocks.

    -

    If you can change simulators, I would recommend QSpice for something like this. It makes it _very_ easy to add digital code blocks to support pretty much anything you'd like to model. Recently, I needed a non-existent Cuk controller model, so I just wrote one myself in about an hour from the datasheet specs using C++ code. There are some good videos on youtube showing how to use QSpice to do this kind of thing if you want to try that route.

    Either way you go, building a model like that will take a bit of work and ingenuity. Since the part is no longer offered by TI, we don't support it, but I think you can find some people on sites like Reddit (r/AskElectronics) and other corners of the internet that still have experience with older parts like this.

    Good luck with your project!